Welcome to Onshape’s Introduction to CAD. Our goal with this course is to teach anyone who is dedicated to learning computer aided design, everything he or she needs to be productive in Onshape, without requiring any previous CAD knowledge.
First, let’s talk about what you will learn and how the lessons are structured. This course is broken down into five main lessons:
The first lesson goes over CAD vocabulary and gives an overview of the Onshape interface and functionality, as well as introduces you to creating sketch geometry. Next, the second lesson focuses on creating basic three-dimensional features, such as Revolve. The third lesson focuses on part design, which teaches how to develop a strategy for combining features into making a final part. From here, the fourth lesson takes a look at creating assemblies, which enable models to have mechanical motion. Lastly, the fifth lesson dives into editing models in a collaborative environment.
Now, for the lesson structure. Each of the lessons contains three main elements. The first element is a set of videos that walks you through each concept. These video concepts often build on one another, making it advantageous to view each video sequentially. After watching all of the videos, you get to practice what you learned with hands-on exercises. Each exercise provides you with a link to a public Onshape document which you must make your own copy of to work off of. These exercises allows you to refine your understanding of the tools and master the concepts. Finally, a short quiz helps you assess how well you retained the information taught in the videos and exercises. If you don’t get all the questions right the first time, don’t worry. Mastering CAD concepts takes time and the best way to improve is to practice.
Remember to give yourself a break in between lessons and make sure you have the concepts down before moving on to the next. If you have any questions or get stuck, check out our forums and get help from the Onshape community. We hope that after taking this course, you will have no problem creating sketches, parts, and assemblies, and will be able to take full advantage of Onshape’s unique collaborative tools. Good luck and have fun!
Welcome to Onshape – Software Overview & User Interface Tour
Let’s take a high level look at some of the key elements of Onshape.
Because Onshape is a cloud based technology, you never have to install any software, plugins, or worry about complicated licensing. Just login from any device with any web browser.
When you do, you will see the documents page which is a home for your designs and documents. Here, you can search for existing documents “create a new” document, upload a document, or just click on an existing document to open it.
You should find the user interface in Onshape very familiar and comfortable. With intuitive icons for commands on the toolbar, a features list that stores all of the sketches, features, and parts in your design, an abundant graphics area, and a view cube to change view orientation. Of course, you can use the center mouse button to pan and zoom….and rotate with the right mouse button.
Onshape provides powerful parametric and direct editing capabilities which we’ll explore in depth in other videos, but I would like to point out that as I make a change here…notice there is no save button anywhere on the screen. The reason is, each action you perform in your designs in Onshape is saved automatically. You can close the browser at any time, or even in case you happen to lose an internet connection, all of your work is stored all of the time.
Another innovation in Onshape is the idea of having parts, assemblies, and drawings all within a single document. Notice there are tabs here at the bottom the document. These tabs are where you can include Part Studios, Assemblies, and Drawings within the overall document in Onshape. By clicking the plus icon, you can add as many tabs as you need. As you can see here, Parts studios are not limited to single parts. In fact, multi-part design is an expected workflow here in the part studio environment, where you can create the geometry for all components without having to worry about external references or complex file structures. With your parts designed in part studios, assemblies are where you can do things like adding mates and creating motion in your designs.
Since designs are rarely done in a vacuum, collaboration is another key element of Onshape, and is something that is quite revolutionary compared with traditional cad tools. In fact, here I can see a colleague has opened this same document. Onshape enables designers, or even entire design teams, to work simultaneously on the same design in real-time. Here I can see my colleague made a change, and of course I can edit any aspect of the design and they will see my changes in real time on their screen as well.
In addition to real-time simultaneous editing, Onshape also provides a powerful branch editing capabilities. At any time you can save a version of a design, which you can think of like saving a snapshot of the design in its current form, but what take this functionality to the next level is the ability for anyone working on the design to branch off of any version to iterate the design or flush out alternative concepts, and then merge any of those branches back in to the design. These branching and merging capabilities in Onshape allow for parallel collaboration and the ability to combine the changes back together.
We will go over all of these topics I mentioned here in depth in upcoming videos, but for now, I hope this gave you a nice primer so you’re ready to take a deeper dive into the tools, techniques and technologies here in Onshape.
Parametric Modeling and Feature-Based Modeling
Before we get into the specific tools and features you will be using, let's take a high-level conceptual look at how the software behaves, which will relate directly to certain approaches and design strategies you'll use once you start building your own models. The three main things I want you to be aware of is that Onshape is parametric, it's feature-based (or in other words history-based, which we'll get into in a moment), and it enables you to establish something called "design intent". So let's take a minute to talk through each of these concepts....
Let’s begin by diving into the concept of parametric modeling. Parametric modeling is based on the idea that your design is driven by specific input values, which you create. Every model created in Onshape is driven by parameters, such as numerical values or certain geometric relationships, in order to control the shape of the model. Dimensions are one type of parametric data. Dimensions control the size and position of sketch geometry and can also be used to relate existing geometry in a model. For instance if I edit the first sketch in this part…..
a number of dimensions appear, all of which can be edited directly in the graphics area. All of the dimensions here control the size and shape of the model. As soon as I make a change to one of these dimensions…..the geometry updates.
Another aspect of parametric modeling involves applying “constraints” to sketch entities. Constraints enable you to create relationships between geometry. For example, if I edit the same sketch I was just working on…..I can bring up the constraints applied to a sketch entity by hovering over it.
This line currently has two tangent constraints applied to it, which forces the line to always remain tangent to both circles. If either of the circles changes in size, the line will remain tangent. This ensures that any features created with this tangent line will maintain tangency. ….. Instead of recreating the dimension in order to resize the circle, I’ll use an equal relation to set the diameter of this circle equal to the inner circle on the left. ….. Now the diameters of these circles will always be equal, even with a dimension change.
Now that we’ve looked at some parameters in sketches, let’s take a look at some parameters in features, like the extrude feature that gives this 2D sketch its depth. If I edit the first Extrude feature …..I can see that it was specified to have a thickness of point two-five inches. If I make a change to this parameter…..
this feature and all associated features update based on the new value.
Another parameter found in features control is something called an “end condition”. The End condition parameter in an extrude feature like this controls its depth. This feature is using what is called a “Blind” end condition, which you can think of as a fixed-depth extending in a single direction. But what if the thickness of the rest of the part changes? Perhaps the intent of this design is to have both of the cylinders always be at the same height….. If I switch the end condition to “Up to Surface”…..I can select an existing face in the part and the feature’s depth will extrude up until it reaches that face, no matter where the face is positioned.
In the case of features that remove material, you can also choose to use a blind end condition, or “up to surface”, or you can even choose something like through-all, that ensures it will remove material regardless of how thick the part gets if you make changes later.
At this point, let’s move on and discuss the idea of feature-based modeling in Onshape.
Regardless of how simple or complex a model is, it is really just a series of basic features that either add or remove material to get to the finished design. All of the features are found in the features list on the left. As you create models in Onshape, every feature you add will be stored here from top to bottom. Using the rollback bar I can step through the features that were used to build this model. As I step through each feature, notice that the model is made up of simple geometry with detail added over time. This process breaks down complicated models into bite-size steps, making it much more understandable. ….. At any time you can edit the 2D sketches….or 3D features. Additionally, Onshape has the power to re-order the features in the list. For instance if I move the feature “Extrude Four”, which is the rod protruding through rotor in the center, above “Extrude Two”, which is the cut feature going into the top of the rotor…..
you can see that the rod no longer protrudes into the rotor because the cut feature removed material from the rod. Two additional parts were also created in the process. Since Onshape is a history-based system, the order of the features in the list impacts the design since each feature is applied in order from top to bottom.
Parametric modeling and feature-based modeling are two of the most powerful tools available in Onshape. They are crucial components in the design experience, especially when discussing the topic of “design intent” in a later lesson.
Let’s take a look at one of the most important concepts when designing in a parametric environment: “design intent”. Design intent is essentially the modeling strategy you employ to create your designs, whether it’s choosing to use one feature type over another to achieve a particular result, or perhaps a dimensioning strategy in a sketch which makes the model behave a certain way if changes are made later.
Let’s first look at how dimensioning schemes can affect a model’s design intent.
If you take a look at the sketch used for this cutout, the current position of the port is the same in all three, however the first set of dimensions positions the port using the left and bottom edges of the model…..the second set of dimensions uses the bottom edge along with a vertical construction line to constrain it to be centered from side to side…..and the third set of dimensions uses the same vertical construction line along with a dimension set below the horizontal mid-line. As this relates to design intent, you will want to think about the results of these dimension schemes in case the size or shape of the rest of the part were to ever change. Each of these will behave a bit differently.
When the size changed, the first example kept the port positioned in the lower left corner…..the second model kept the port horizontally centered but toward the bottom edge…..and the third model kept the port horizontally centered but higher up toward the center of the face. It takes time to understand exactly how to dimension your sketches to get the right design intent, but don’t worry, you can always go back and make edits later on if something updates unexpectedly. In fact, experimentation with dimension schemes is one of the best ways to improve your understanding of design intent.
Earlier I mentioned how you might choose one feature type over another to achieve the same shape. Let’s take a look.
In this example the main body of this headphone has three concentric cylinders connected together. These were created using a series of individual extrude features that stack on one another. ….. This means that the design intent is determined by each one of these individual features. If one of the cylinders changes in depth…..
the positions of the other cylinders are affected due to being stacked.
If I bring up another example, you can see a single revolve feature was used to get the same shape. The depth and diameter of each cylinder is controlled by the sketch profile of the revolve feature. This means that the sketch must be modified in order to make the same change. One potential advantage of this approach is that a slight change to the sketch profile can be made to alter the model geometry, and a change like this one might have been more difficult to do in the other example that used stacked extrudes.
Before wrapping up, let’s just take a quick example of how design intent can be incorporated when there are several parts that make up the same design. This part studio has four dowels passing through a slider. If the size of the slider is modified…..
not only do the dowels reposition, but the two endplates also change in size. This means that the geometry of the other parts link back to the driving dimensions found in the slider. This is due to “Sketch Two” ensuring that the circular cutouts are point one five inches away from the edges…..as well as “sketch seven” projecting the circular cutouts from the slider onto the endplate. ….. This shows you how significantly the model geometry can change by editing a single dimension value.
Design intent is incredibly powerful in a parametric CAD environment. But in case you’re worried about fully understanding how design intent impacts your current models, I assure you that it comes naturally as you create designs. Just be sure to give some thought about an approach and strategy for creating your models, as well as the dimension schemes and relationships that will be applied. Once you’ve done that, you’re modeling skills will take off and you’ll find new confidence in how well you can model!
Sketches are at the core of any 3D design you create. If you have been using 3D CAD, but are new to Onshape, the picks and clicks you might be used to in other programs are similar here, but there are some that are unique to Onshape. Let’s take a few minutes to go over a few of the sketch tools used most often so you feel nimble in the sketch environment.
To start a sketch you can of course click the Sketch icon and then choose a sketch plane…..but a nice shortcut is to simply right click on any plane or face…choose "New Sketch"……right click again and you can view normal to the sketch plane. Any time you see this pop-up window, this lets you know you are editing a sketch.
The line command lets you quickly create a chain of lines to create a profile. Notice as add this third line segment the profile becomes shaded letting me know I have an enclosed region that could be used for an extrude or other 3d features. I didn’t have to create an additional line segment to close the profile here since Onshape treats this existing model edge as a boundary for the profile. To turn off the line I can right click and select “Escape Line”, or just press escape on the keyboard. You can also create single lines without a chain by clicking to start a line, and with the mouse button still depressed, release the mouse at the spot you would like to end it.
Line segments can be toggled to construction by selecting them, and pressing the construction icon on the toolbar. I’ll go ahead and make this line vertical as well. Sketch tools such as rectangles, circles and arcs have a flyout menu allowing you to select the different methods of creating those entities but I’ll skip over those, as well as the spline tool for now.
Sketch fillets are another sketch tool you will most likely use often as well. Here you can select any two intersecting line segments, or a vertex. With your selections made, just type in a radius.
The offset sketch tool works as you might expect, but there are a few picks and clicks here that you should be aware of. With the tool active, just click any line segment, or combination of segments that you wish to offset….and with your selections made, you can use the arrow in the graphics area to specify the direction. To enter the offset distance, just click anywhere to make the pop up appear where you can type in the distance.
The “Use” command allows you to convert any model face or edge into sketch entities on the plane you’re working with.
And finally, the last sketch tool I’ll go over here is the trim command. The trim command is simple. Just click any entity that you would like to get rid of, and it is trimmed back to the closest intersection.
At this point, I could click the extrude icon to create a 3d feature, or just click the green check to save and exit the sketch. When I do the sketch popup disappears, and as with any item in the features list, to make changes, just double click on it and the sketch popup reappears.
Before wrapping up, there’s one last thing I’d like to mention. You may have noticed as I was selecting items, that there was no need to hold down the control key to select multiple items. This is the case with everything you do in Onshape. Anything you click on becomes selected, whether its sketch entities, model faces, or even items in the features list. To clear your active selections, just click again anywhere in white space. In case you would like to window-select anything, you can press the alt key on the keyboard while dragging the mouse.
Dimensions and Constraints
In parametric modeling, dimensions and constraints are they key to establishing predictable and powerful design intent as you create sketches. The tools and techniques for defining sketches in Onshape are straightforward. Let’s take a quick look.
As you sketch geometry, constraints are added automatically, as you can tell by the snapping behavior when a line segment is created close to vertical or horizontal. You can also wake up inferences to other geometry simply by hovering your pointer over it, such as this line segment, or even wake up additional inferences such as this point, so that this next endpoint of the line can be horizontal to the point, ….parallel to the segment…..or even perpendicular to the segment, while maintaining the horizontal constraint.
I’ll escape out of the line for a moment. You can always see what constraints have been added to any sketch entity simply by clicking on it…and a small flag appears. When I roll over the flag you can see the geometry highlight that has the constraint applied. To remove a constraint you can just press delete on the keyboard while the constraint flag is selected. I’ll click undo twice to bring back the constraint….and I’ll reactivate the line sketch tool by clicking the icon on the toolbar. Automatic constraints are usually a convenient way to build in design intent while you sketch, but in case you ever want to avoid having the constraint added while you sketch, you can hold down the shift key on the keyboard when you click…..and you can see that no constraints were added. You can of course add constraints manually by clicking on any geometry….and using the constraint icons on the toolbar.
I’ll go ahead and add a circle to this sketch….using an automatic midpoint constraint as you can see by the cursor feedback….and I’ll make the two perpendicular lines equal length.
The colors of sketch entities let you know what is fully defined or underdefined. Blue geometry is free to move, while black geometry is defined by either constraints or dimensions. That said let’s go ahead and add some dimensions here to fully define this sketch.
Dimensions are added by clicking on any combination of lines, points, circles, arcs, etcetera, but before I type in a value here, I would like to point out a nice behavior here in Onshape….the first dimension you add to a sketch automatically scales the entire sketch. If you’ve ever created a sketch in other CAD systems and the items you sketched were significantly smaller or larger than the dimension value you added, you can probably relate to what a nice feature this is, and as you can see, all of the geometry and constraints behave predictably.
You can always come back to make changes simply by double clicking it, or in case you wish to delete the dimension, you can click on its leader lines to select it, and press delete on the keyboard. Point to point dimensions can be added as vertical, true length, or horizontal by moving your pointer to the different positions….click again to place it, and type in a value.
I’ll add a couple more dimensions here…..and finally when the sketch turns completely black you know it is fully defined. Just so you know, when you’re dimensioning a circle, Onshape will add a diameter dimension. If it’s an arc, Onshape adds a radius dimension to the geometry. Before wrapping up, let’s take a quick look at what happens when you over-constrain the sketch. When I add one more dimensions here, when I click to place it…..some items in the sketch turn red. What’s nice about this is that only the conflicting items turn red, so you can make an easy decision about what to keep and what to get rid of without troubleshooting the sketch to figure out what the problem is. I’ll get rid if this dimension….and the sketch is now fully defined.
Extrude is one of, if not the most common sketch based feature used in 3D modeling. Let’s take a look at how it works here in Onshape. Here I have a sketch prepared with a handful of closed profile shapes. Sketches containing many profiles are incredibly common in Onshape, allowing you to intuitively sketch the shape you’re looking for, plus any details you wish, and use just portions of the sketch for any 3D feature, whether it’s for adding or removing geometry.
When I click the "Extrude" icon, a popup appears where you can define the options and parameters for the feature. Here I can select any regions of the sketch…and by default a "Blind" end condition is selected where I can enter a value….flip the direction…or use the arrow in the graphics area. Of course, there are also other end conditions such as "Symmetric"…."Up to next," "Up to surface," etcetera. For now, I’ll set it to "Blind"…and enter a value.
The extrude command is powerful in that you can accomplish quite a few outcomes from the single command. For instance the "Add" and "Remove" options, as you would expect will either add material or remove material to the part you’re working with. If I add this additional contour to the selection window you can how the remove option makes a cut into the part. The "Intersect" option leaves you with just the intersecting geometry, which can be extremely powerful in certain design approaches….and the “New” option will result in an additional body, and in the case of Onshape a new part here in this part studio. For now, I’ll use the add option.
In this next field below, you can specify what this new geometry will be merged with, which comes into play much more when taking using a multipart design approach, but in this case, since this part studio only contains a single part, that’s what this extrude will be merged with.
Take a look here at the preview slider. As I slide it from one end to the other you can see how the preview goes from transparent to opaque, which allows you to quickly visualize the before and after of the feature you’re creating. You can also specify whether you’d like to extrude the profile as a "Solid" or a "Surface." For this feature, I’d like to create the extrude as a solid. At this point I’ll click OK, and the extrude is added to the features list. I’ll go ahead and rename it…
Next, to make a counterbore hole here, I can reuse another contour from this same sketch. I’ll launch the "Extrude" command…and I’ll select the circular profile. This time, I’ll select the "Remove" option…and for the end condition I do have the option for “Through All” available which would cut through the entire part, but I’ll again set this to "Blind" and enter a value. At this point I can hide the sketch….and rename the cut I just made. As with any feature or sketch in Onshape, you can always come back to make change simply by double clicking on it in the features list.
The revolve is another essential tool in your arsenal for 3d design. The revolve command can be found right next to the extrude icon on the toolbar. In the pop-up, I can choose whether I’d like to create the revolve as a solid or a surface. I’ll choose solid. Next, I can select any sketch profiles, faces, or edges that I’d like to revolve. I’ll select this sketch profile I prepared ahead of time.
To select the revolve axis, I can activate the selection field….and as a side note, you can always tell which field is active by the blue highlight. The axis can of course be any model edge, line segment, or a centerline like I have in this case. As soon as I click it, the preview appears. The default option here is “Full” meaning a full 360 degree revolution, but I can set this to one direction with a specified value. With this option enabled I can also use the flip direction arrow, or use the icon in the graphics area to drag it manually. Symmetric will split the revolve evenly about the sketch plane…and “two directions” provides independent control of the revolve on either side of the sketch plane.
I’ll set it back to “Full”, and before clicking OK I want to pay attention to the options above.
I would like this feature to result in a new part being added here in the part studio, rather than merging with the existing geometry, so to do this, I’ll use the “New” option, and right away you can see the preview appears in a different color as a visual indicator that it will be its own part. When I click OK, the revolve is complete and listed in the Feature list, as well as in the parts list. It never hurts to rename any features or parts to make them easy to identify later.
Sweeps are another powerful parametric feature in Onshape. The only requirement for a sweep is that you must have geometry for the sweep profile and sweep path. You can use any existing model faces and edges for both the profile and path, but in this case, I set up a couple more sketches ahead of time so we can take a look at a few options and techniques.
I’ll go ahead and launch the sweep command, using this icon. The options for a sweep are simple. The first selection I need to make is to choose whether I’d like to create the sweep as a solid or a surface. I’ll choose a solid. Next, I’ll select the faces or edges to be used as the profile. I’ll select the sketch profile….and for the sweep path, I just have to click in the window to activate the field…and I can select one of the line segments. With the profile and path selected, I can choose wither I’d like to create this sweep as a new part, or Add, Remove, or Intersect it with existing geometry like you saw with the extrude and revolve features. I’ll choose Add, and then use the Merge Scope selection box to choose the body to add it to…..in this case the circular extrude. When I click the check, the weep is completed. I’ll show the sketch used for the path again, and click the sweep icon to create a second sweep here. This time, instead of using a sketch for the profile, I’ll select this face belonging to the first sweep. And for the path, I’ll select this other arc. I can create this as a new sweep, and when I click the green check, you can see this time, the sweep is created as its own separate part and is listed in the tree. At this point each of these parts could be modified independently, such as applying fillets or shells, which can provide nice flexibility, particularly with complex designs. To combine these parts into a single part, this can be accomplished quickly and easily using the Boolean command. I could use the union option to join the parts together, but instead ill cancel out and simply double click the sweep feature to edit it and change it to Add. I’ll check to box to simply merge with all intersecting geometry, and click the check to complete the sweep.
And with the sweeps and original extrude feature merged into a single body I can do things like adding fillets, maybe a shell, or any number of applied features that we will cover in depth in another video.
Fillet & Chamfer
Fillets and Chamfers are easy and intuitive to apply to your models in Onshape. The fillet and chamfer icons are grouped together on the toolbar next to other applied features like draft and shell, which we’ll cover in another video. Let’s look at the fillet first.
In the popup, you can select any edges or faces of the model…and with the selection box still active you can continue making selections, or to deselect an item, you can click the red X in the window, ….or just click on it again graphically. I’ll go ahead and type in a radius.
Onshape also supports Conic fillets, which are incredibly useful when styling and aesthetics are important, giving you much more control over the resulting curvature. Without this option enabled you will get a standard, circular shaped constant radius fillet, or, when you enable it, you can enter a Rho value to define the curvature. In case conic fillets are new to you, a Rho value set to point 5 will result in a parabolic curvature …..less than point 5 will result in a more elliptical shape….and a value greater than point five will result in a hyperbolic shape. I’ll go ahead and click OK to finish.
Let’s add another fillet feature to break some other edges here. Because the tangent propagation option is enabled, it’s easy to make selections to pick up the surrounding sharp edges. I’ll click OK, and the feature is added. In case you need to make any adjustments, you can always double click the feature in the feature list to bring back the same options, where you can change the value, or add or remove any of your selections.
At this point, let’s change gears for a minute and take a quick look at the chamfer feature.
I’ll go ahead and launch the chamfer command. The options for the chamfer are very similar to what you saw with the fillet. The tangent propagation option makes it easy to make edge or face selections. I’ll enter a distance value, and I can choose to make this distance equal in both directions……Or I can specify a distance in two directions…….or I can choose to use a distance and an angle value. If I choose to mke the distance equal in two directions, the chamfer angle will be equal to 45 degrees.
I’ll go ahead and add another chamfer feature, and I’ll select this face so that the chamfer will be applied to the hole on both sides….and I’ll add one more….to the edges of these holes on top.
Draft & Shell
Draft and Shell features are other common features that you will apply to your models, particularly when designing plastic or molded parts. The icons are grouped together on the toolbar with other applied features, and we’ll start by looking at the shell feature.
The options for the shell are straightforward. Type in a wall thickness….and in the “faces to shell” selection window, you can pick any faces that you would like to remove. When I click OK, the feature is added. Of course, any time you are applying shell, or draft features for that matter, the order in which you apply them is important since it has such a significant impact on the resulting geometry. In this case, I should have applied the shell command before all of these vents.
Since Onshape is a history-based system, the fix here is simple. I can just click and drag the feature in the feature list to move it up before the vents.
Let’s switch over to another example.
In cases where you need to apply a slope to faces of your models, the Draft feature is what you will use. Before I launch the command, let me roll back in the feature list.
The draft command has fields for Neutral Plane, and Entities to Draft. The neutral plane, is the plane or surface that will determine the direction of the draft angle. I’ll select this face……and for the entities to draft, I’ll select these outer faces. I’ll type in a draft angle of 6 degrees….and you can always use the “opposite direction” button to change the draft from going outward ….or inward from the neutral plane. The preview slider can also be useful here to visualize the results. I’ll click OK and the feature is added.
At this point I’ll roll to the end of the features list to show you one more helpful option with the draft. I’ll use the same face as the neutral plane….and again use 6 degrees, but before I select anything, notice the draft feature also includes an option for tangent propagation. Because of the fillets here, the tangent propagation option makes it incredibly easy to apply the draft to the remaining interior faces.
In addition to Onshape’s powerful parametric capabilities is a suite of best in class direct-editing tools that enable you to manipulate any geometry you’re working with, whether it’s in your history based models created in Onshape, imported geometry, or a combination of the two like I have here.
The Move Face command contains many of the traditional direct editing capabilities you might expect such as translation, rotation, and offset, so let’s start by quickly going through each of these.
With the translate option enabled, I can select any face or combinations of faces….activate the translation direction field, and choose an edge to define the vector. I can click and drag the arrow graphically….or type in a value.
Let me go ahead and re-launch the move face tool. This time I’ll use the rotate option. Here I can select any face that I wish to rotate…..specify an axis for rotation, and again I can use the manipulator graphically or just type in the angle.
The offset option can produce similar results as the translate option if you select planar faces, but this option is typically used for non-planar faces such as this cylinder, allowing me to type in an offset value to increase or decrease the radius.
Besides “Move Face” there are a few other direct edit commands here on the toolbar. Delete face allows you to remove geometry from the model. In a simple case, I can just select a face to delete…and click the green check….but let’s take a look at a bit more complex geometry. I’ll go ahead and click the delete face icon once more.
If I wanted to get rid of this recess here, which is made up of quite a few faces, Onshape provides a convenient “create selection” tool available from the right click menu. When I select it, the create selection popup appears, and if I expand the drop down you can see there are options for protrusion, pocket, hole, fillets, tangent-connected, and bounded faces.
In this case, I’ll select Pocket….and choose this bottom face of the recess. When I do, you can see 7 entities were selected. I’ll select this filleted face….and now 13 entities are selected. Notice the delete face pop-up still does not have these items listed in the “delete faces” selection window. To add them, I just have to click “Add selections”. When I do, I can close the create selections popup …..and I’ll click the green check and the pocket faces are deleted.
Let’s take a look at one more direct editing tool, Replace Face. The replace face command is powerful tool with many applications. It is essentially a way to trim or extend an existing face to a new surface. I went ahead and created a surface ahead of time which I’ll go ahead and show in the document. When I launch “replace face”….here I can select which face I would like to replace, or in other words trim or extend….and the surface to replace it with. There is an option to offset along with the offset direction, but I’ll leave this at its defaults and click OK….and I’ll go ahead and hide the surface body.
Starting a Design
Beginning to create a new design can feel like a challenging task, especially if you are just starting to develop your CAD skills. However I want to remind you that even the most complicated models begin with a single feature, which is often a very simple shape. Even this engine housing, which has a number of complicated features, began with a single revolve feature. …..
and as I include more of the features back into the part…..you can see that even the most complex designs are often just a combination of relatively simple features. And in the end…..a great design emerges.
Let’s take a closer look at one of the components in this concept vehicle. The suspension mount shown here connects four shock absorbers on each side of the vehicle, two of which have collars that connect to additional hydraulics. This requires the part to have at least six holes for the shocks and hydraulics to connect to it. Additionally, since the hydraulics are in-line with the shock absorbers, a cutout was created so that the hydraulics could reach over the top of the mount and connect at the center. ….. Now that many of the important features have been identified, I’ll switch over to the individual part in a separate tab to begin walking through the design process.
When deciding how to begin creating a part, the first step is to identify which plane to sketch on. In order to make this decision, there must be some foresight into how the features will be created from the sketch. In this part I can see that many of the profiles have the same cross-section in the Y-direction…..
which means that these extrude features were created on planes that extrude in the same direction. Another way of describing this is saying that these planes are “normal to the Y-axis”. To help illustrate the idea of a plane being normal to an axis, think of a pencil poking straight through a piece of paper. In that case, the paper is the plane and the pencil is the “axis normal to the plane”. ….. With this understanding, the first sketch can be created on the Front plane, which is also normal to the Y-axis.
To begin working with the first sketch I’ll rollback in the features list. The bar shown here in the list can be moved around and allows for the model to exist in a state where only the features above the bar are active in the model. So if I roll it back so only the first sketch is above the bar…..and make sure it’s visible in the graphics area. …..
you can see the sketch on its own with no other features. We will use this tool throughout this lesson to show what features were added to the model.
Notice that the sketch has multiple overlapping sketch entities, such as the angled edges extending into the circles. This allows for specific sketch faces to be used in the extrude feature. When I roll the bar forward one step in the features list…..
you can see that the feature was created with the holes already cut out. If I edit the feature…..you can see that these sketch faces were not selected when the feature was created. Additionally, the feature was created symmetrically about the Front plane, extruding the feature two inches from the plane in both directions. This is an important design choice that will come into play later on when creating other features.
Now the second feature can be created. But which feature should I create next? There are a number of options available, however I’ll use the design strategy that larger features should be created first, and then smaller features created after. Following this design strategy, I will create the cutout that allows the hydraulics to reach over the top of the part, which is the next largest feature. If I roll down in the features list…..
the sketch was created on the front face of the part, which will allow the extrude feature to cut back into the part. This face is normal to the Y-axis, which will cut into the part in the Y-direction. If I roll forward in the features list…..
You can see the feature cut into the part to a certain depth. If I edit the feature…..
you can see a “Blind” end condition is used to cut into the part by three inches.
The third feature to add to the part creates the cutouts for the shock absorbers. If I roll forward in the features list…..
notice that the circular sketches that create the cutouts do not lie on a specific face. In fact, this sketch was created on the Front plane. ….. This allows me to cut symmetrically, which ties back to the first symmetric extrude feature. If I roll down in the features list…..and view the part from the Right plane…..
I can see that the cut exists in the center of the part, and that the tabs that connect to the shock absorber have equal thicknesses on either side of the cutout.
Finally, I can add the holes for the hydraulics. If I roll forward in the features list…..
you can see that the sketch for this feature is created on the face of the part created by the larger extruded cut. Now if I roll forward once more in the features list…..
the holes are added to the part. This completes creating all of the part geometry.
To review the design approach, this part only required four features in order to create all of the necessary geometry. This was accomplished by choosing strategic sketch planes and faces - such as the front plane - to create extrudes that added and removed material. In addition, the design process was sped up by utilizing the “symmetric” end condition for some of the extrude features. This allowed for a relatively simple and functional part to be created with a very short list of sketches and features.
All in all you've seen that creating complex parts is all about breaking it down into smaller features. A great design method is to create the biggest features first and work down to more detailed features, until the model looks just right.
Basic Part Design Example
Whenever you begin creating a model in Onshape, decisions have to be made about which planes to sketch on, which directions features will extrude, and in which order to create the features. This all ties back to design intent, which if planned out correctly, will speed up your design process once you have a vision for the model.
The model shown here contains a number of parts that form a functioning fuel valve actuator. ….. I’ll walk through how to create this adapter shown here. If I switch over to the next tab in the document…..you can see the part shown individually.
The first thing I want to do is develop a design strategy for creating the part. This will involve determining which features are ”biggest” and drive the rest of the part. I’ll start with these features and continue to add more and more detail as I go. First I notice that the profile with the five holes on the right side of the part has a continuous cross section in the x-direction. ….. This means that I can create this portion of the part first using a single extrude feature. Next I notice the feature extending out of the back of the part. This feature joins the first extrusion at the center, which means that the first extrusion should be created symmetrically about the sketch plane in both directions. This can be accomplished by creating the first sketch of the model on the right plane and then extruding using a “symmetric” end condition. Then I’ll create this second extrusion on the back of the part. Once all of the features that add material to the part are created, I’ll create features that cut away material, such as the angled face here on the part. Once the major part geometry has been created, I’ll add holes and indents in the part. Lastly I’ll smooth out edges using fillets where necessary. ….. Now that a design strategy is in place, let’s switch over to another tab to begin creating the part.
You can see a couple sketches shown here that will be used to create the part. The first sketch, which is currently shown on the right plane, was created by projecting the front face of the threaded fitting. …..
The other sketch was created on a plane offset from the front plane. To begin creating the part I’ll create an extrude feature…..which will be a new part…..select all of the faces in the sketch…..change the end condition to “symmetric”…..and then set the depth to one inch. …..
Now I’ll create the other extrude on the back of the part. Instead of creating a new part I want it to be added to the existing part…..then select all of the faces in the sketch…..make sure the end condition is set to “Blind”…..using a depth of point six two five inches…..and make sure that the feature merges with the existing part.
At this point I have the rough geometry of the part, but obviously there is a lot more detail to add. I can now begin removing material. The section of removed material will create angled faces on the slot-shaped extrude. I can create this cut in a single feature using a “through all” type cut. This means that the sketch for the cut needs to be positioned so that it can cut through all of the geometry in a single direction. I’ll use the side face of the part to create the angled face…..then project all of the vertical edges of the slot-shaped extrude…..draw horizontal lines connected to the endpoints at the top and the bottom…..and then draw angled lines to create the angled faces. ….. I’ll make sure that both faces have 45 degree angles…..
and now I can create the cut through the part. I’ll select both triangular faces…..make sure the feature is set to “remove” material…..use a “through all” end condition…..in the correct direction…..and merge it with the part.
Now I can begin adding holes and indents to the part. To begin creating the holes on the sides of the part I’ll create a sketch and project the sketch entities…..on both sides of the part…..and I’ll create the first hole through the center of the entire part using the inner circular sketch face. …..
Now I’ll add the indent features. I’ll create a blind cut on the right side of the part…..using the inner face between the two circles…..with a depth of point zero two inches…..and I’ll repeat this on the other side of the part. …..
Now I’ll add the holes in each corner of the side faces. ….. I’ll select all four circles as the sketch faces…..and instead of doing a blind cut I’ll make sure that the holes stop as soon as they meet the faces of the slot-shaped extrude in the back. This means that an “Up to Surface” end condition needs to be used…..and I’ll select the side face of the slot-shaped extrude for the holes to stop. ….. I’ll repeat this again on the other side of the part. …..
Before moving on I’ll hide all of these sketches.
The last holes that need to be created go through the slot-shaped extrude. All three holes stop when they meet the next face in the part, which means I can use an “Up to Next” end condition. I’ll select the three holes as the sketch faces…..change the end condition to “Up to Next”…..and make sure it’s going in the right direction.
To wrap up creating the part geometry I’ll add some fillets. It is common practice to add fillets at the very end of modeling a part. All of the fillets will have a radius of point zero six three inches…..and I’ll make sure “Tangent Propagation” is turned on for tangent edges to be selected. I’ll begin selecting edges that join the slot-shaped extrude to the main body of the part…..but notice that when I select the edge of the angled face the preview disappears. This is because not all of the fillet geometry cannot be created in a single feature. I’ll delete this edge from the feature…..and select the rest of the edges to complete the feature. …..
Now I can create the remaining fillets in a second feature. These fillets will have the same radius…..and I’ll select the edges along the angled faces. …..
This completes adding all of the necessary features to create the part geometry.
To wrap up, let’s recap the design strategy taken to create the part. First, the sketches were created on the appropriate sketch planes in order to extrude in the correct directions. Then all extrudes were created that add material. Then all extrudes that remove material were created, including indents and holes. Many of these had different end conditions, which depended on the existing part geometry. Finally, fillets were added to the appropriate edges, which required multiple fillet features to account for all of the edges. This design strategy is a great starting point for many of your designs, and will enable you to create robust, well-designed models moving forward.
Machine Part Design Case Study
Let’s get some practice designing a machined part like the one you see here. You can see that for the most part it is made up of extrude features which added the geometry and removed geometry for the pockets and cuts, as well as some fillets to break the sharp edges. Let me switch over to this other part studio to get started.
For this example I have a sketch already created. The two dimensional geometry here can be created in Onshape using the various sketch tools and constraints… but for this example I would like to show you how you can leverage a sketch like this that contains multiple sketch profiles to create the 3D geometry for the part using various features
To get started, I’ll extrude the main body of the part. I’ll make sure all of the sketched geometry is de-selected and select the Extrude icon from the toolbar.
I’ll select the interior profiles to create the geometry for the body of this part…. And I’ll extrude to a blind depth of thirty millimeters.
I’ll click OK and the first extrude is complete.
I’d like to make sure that the sketch is “shown” from the feature list so the sketch profiles can be used in the upcoming features I’d like to add.
Now I’ll make a quick adjustment to the overall profile and round out the sharp corners where the two round profiles meet. To do this, I’ll use a Fillet…. I’ll select the Fillet icon from the toolbar…. select both of the vertical edges… then set the radius to twenty five millimeters. And when I click OK, the fillets are added, rounding out the shape of this feature. Keep in mind that these fillets could have easily been added to the original sketch profile saving a little time, and reducing the amount of features in the part, but either approach works fine.
Next, I’d like to extrude the sketch to create the mounting tabs. I’ll click the icon for Extrude… make sure that the option is set to “Add” so material is added to this part, and then pick the six profiles for each of the tabs and the corresponding circular profiles. I’ll be sure not to select the interior profiles so the mounting holes remain in place. This extrude will be at a depth of ten millimeters… I’ll click OK to accept the extruded mounting tabs.
For the next feature, I’d like to add the web surrounding the tabs. To do this I’ll use the outermost profiles of the sketch, so I’ll click the Extrude icon once again and then select each of the four outer profiles. I’d like to set this depth to five millimeters…. and I’ll click OK to finish.
With the basic shape extruded, I’d like to start removing material to create the through holes and pockets in the part. I’ll begin with another Extrude feature, so I’ll click the icon and this time make sure to select the “Remove” option. I’ll flip the part to get a better view of the sketch and select the interior circular profiles.
Keep in mind that any sketch geometry that intersects will create separate closed profiles, so I’ll be careful to select all of the profiles required for the shape that I want.
I’d like to remove material so I’ll make sure that the Extrude is in the correct direction and remove a blind depth of twelve millimeters. I’ll click OK and the material is removed.
For the next feature in this part, I’d like to remove material from the top face. So I’ll create a new sketch on this face…. Then use geometry from the previous sketch and project it onto this new plane. … Right click, and select “Use”. <de-select sketch>
With the new sketch complete, I’ll use the Extrude icon once again to remove the material. I’ll select this new profile and set the depth to fifteen millimeters. I’ll click OK and the material has been removed from the top face of the part.
At this point, I’d like to create a through hole using another circular profile. I’ll rotate the part to get a better view of the original sketch on the bottom of the part, and I’ll select the Extrude icon. This profile will be a “through all” end type. I’ll select the circular profile… click OK… and the cut is added.
<Switch to Isometric>
With the majority of the geometry complete, I’d like to add some fillets to the sharp corners of this part. I’ll click the fillet icon and add one millimeter fillets to edges on the top of this part... Keep in mind that multiple fillet features may be required to produce the results you want, especially in cases where you have overlapping fillet geometry. A couple of rules of thumb to keep in mind with fillets, and you might already be familiar with these from working with other parametric, history based CAD systems. But, generally speaking you want to save cosmetic fillets toward the end of the part, work on larger fillets before smaller fillets, and try to keep fillets that are the same size within the same fillet feature, rather than having a bunch of fillet features in the features list that have the same value.
To finish up, I’ll just hide the sketch from the workspace… give this part a name <Gear Housing>…. and we’re done.
In this exercise I created most of this part from a single sketch, and you can see how it’s easy to just select the profile you want for each feature. But as a side note, I could have used portions of this sketch to create the geometry for new parts within the same part studio. For some extra practice, why don’t you try and create a few additional parts here in this design using the same sketch, by using the “New” option for the next Extrude.
Assemblies in Onshape allow you bring in parts from part studios or even sub-assemblies created in other assemblies, and assemble them together using mates to establish behaviors and motion in your designs.
Here you can see this part studio I’m working with has a few parts shown here in the feature list. As you create features, such as an extrude….the options of New and Add allow you to decide whether the feature you’re creating should result in its own part here in the part studio, or if it should merge with an existing part. I’ll select “Add” to have this extrude feature merge with the simplified gear. The multi-part design philosophy in Onshape is powerful because it allows you to build in design intent and relationships with other parts, such as the up to surface end condition to the gasket part, as well as the sketch that’s being used for this extrude being offset from the housing part. Of course, I don’t have to worry about complicated external references since everything exists here in this part studio.
<use up to surface to the gasket>
As you create multiple parts in part studios, it is generally a good practice to rename parts here in the feature list which will make things easier when you insert them into an assembly as you’ll see in a moment.
If you take a look at the tabs I have in this document I’m working with, I have a handful of part studios…and an assembly already created, which contains the parts from another part studio. I also have an empty assembly that I will be working with, but keep in mind you can always create new part studios or assemblies by clicking the plus icon.
Here in this empty assembly , the feature list contains sections for mate features and part instances, and the toolbar has icons to insert parts, as well as adding mates which we’ll cover in another video. When I click the “Insert Parts and Assemblies” icon…..a popup appears. This window allows you to search for items and by default shows a list of all of the items in this document. The filters allow you to isolate part studios or assemblies.
To insert something into the assembly, just click on it. Here I can insert an entire assembly into this assembly ….and notice these other listings show both the name of the part, as well as the name of the part studio where they were created. You can click the part name to insert just that part, or, if you click the studio, all of the items in that studio will be inserted.
Once I’ve made my selections I can just click the green check to close the popup. The feature list shows all of the items I inserted, and notice the assembly I inserted can be expanded to see the parts that belong to it. At the moment everything in this assembly is free to move. You can click and drag an item to move it….or click on it, and use the triad. The triad has handles for translation, ….as well as rotation. Notice when I click on the sub-assembly here, all of the items move together. This is because this sub-assembly has some mates applied that were used for positioning each of its parts, which we’ll cover in depth in another video.
Plastic Design and Consumer Product Case Study
Let’s take a look at an example of a consumer product design by designing the top of cover of this plastic enclosure. By designing the top cover here in this part studio containing the other parts I can use a lot of the existing geometry as a reference to achieve a design intent of the top cover fitting perfectly with the parts it will be mated with.
I’ll start with the lip that will be inset into the bottom cover so I’ll create a new sketch on the inset face…and I’ll look normal to the sketch plane. To have the lip follow the same contour as the lip on the bottom cover I’ll select each edge…..and select “Use” to add these as sketch entities here in this sketch.....and with the items still selected, I’ll go ahead and offset them…toward the inside…..and I’ll use a value of 30 thousandths to match the face of the existing face.
I’ll click Extrude….and use the contour I just created. Since this will be the first feature of the new part, I’ll select “New”…..and for the end condition I’ll change this from Blind, to “up to Surface”….using the top surface of the lower cover….and click OK.
With the new part added in the features list, I’ll go ahead and rename it.
To create the rest of the depth of the top cover I’ll again start a new sketch. Since I’d like the top cover to follow the same contour as the bottom, I’ll select each of the outer edges…..and click “Use”. I’ll click the extrude icon….and since I would like this extrude to merge with the lip I just created, I’ll click Add.
In the “Merge scope” field I’ll select the Top Cover Part from the features list to have this extrude merge with the lip. I’ll use a blind end condition with a depth of .25, and click OK.
Since this will be an injection molded part, I’ll add a draft. To select the neutral plane, I’ll go ahead and hide the bottom cover…and use this face here. For the entities to draft, I can just select one of the outer faces…and because tangent propagation is enabled, you can see in the preview that all of the other faces will be have the draft applied as well. I’ll use 3 degrees….with the draft going inward….and click OK.
Next, I’ll add a chamfer to the top edge….of point two ….. and click OK. To round off the top edge, I’ll add a fillet…of point three five….and click OK.
At this point I have the contour I’d like for the top cover, so let’s go ahead and use the shell command to remove material from the inside and make this a thin walled part. I’ll use a wall thickness of fifty thousandths to match the wall thickness of the bottom cover, and click OK.
Next I’ll add a couple of cutouts here on the top cover to accommodate the button, and a display and power indicator light.
I’ll start a new sketch on the top….and to make the cutout for the button, I’ll select each of its edges…and offset them fifteen thousandths.
For the display, I’ll use a center-point rectangle, positioned directly above the origin…..and I’ll add some fillets…..and I’ll add a few dimensions.
And lastly I’ll add a circle for the power indicator light….and give it some dimensions as well.
At this point I’ll click the Extrude icon…and use the “remove” option to cut away material. For the merge scope, I’ll select the top cover….and I’ll use a through-all end condition……and click OK.
To finish up this example, I would like to add a couple of bosses with alignment pins that go into the bosses on the bottom cover.
I’ll go ahead and start a new sketch on the inside face. I would again like to reuse existing geometry from the bottom cover, so to make my selections, let me go ahead and show the bottom cover…and I’ll hide the top cover I’m working with for a moment.
I’ll select each of the circular edges of the bosses on the bottom cover…and select “Use”.
Now, although I will be adding these extrude features to the top cover, I can go ahead and keep the part hidden to make the selections easy.
I’ll click the extrude icon….and I’ll start with the inner contours for the pins….I’ll use an up to surface end condition so that the pins go all the way to the bottom of the bosses….
For the merge scope I will be sure to select the top cover. When I do, the preview disappears, but this is because I have the top cover hidden from my display at the moment. I’ll click OK and will turn the top cover back on in a moment.
I’ll repeat the process for the outer section of the boss, so I’ll show the sketch I created a moment ago…and for the extrude….I’ll select each contour of the sketch.
I’ll again use an up to surface end condition, this time using the top surface of the boss as the reference.
In the merge scope, I’ll again select the top cover…and the preview will disappear momentarily since I have the top cover hidden to make these selections.
I’ll click OK….and I’ll go ahead and show the top cover….and hide the bottom cover to see the results.
I’ll go ahead and hide the sketch I created a moment ago, and I could of course continue adding additional features, or even create an assembly studio with this design to insert additional components.
Before wrapping up, I would just like to quickly mention that one of the benefits of designing this part here in the part studio is the powerful design intent that was created due to the tight relationships between the geometry in in the top and bottom covers….so if the shape of the bottom cover were to ever change….the top cover will update right along with it.
Medical Device Case Study
Let’s get some practice designing a part in Onshape, then test out the functionality inside of an assembly. In this exercise, I’d like to create a medical device, in this case a replacement hip joint using various modeling techniques and features.
Before getting started, I’d like to change the units in this document to millimeters.
I’ll start by modeling the base, so just like any other part in Onshape, I’ll first create a sketch. I’ll right click on the Top plane and select “New Sketch”… Next, I’ll look normal to the sketch plane and then begin to sketch the profile for this part using circles and lines. I’ll start with a center point circle placed at the origin…. Then place another center point circle coincident to the top of the first circle. Before adding any dimensions here, I’ll finish the geometry and constraints…. I’ll add two lines coincident to the edges of each circular profile…. And with the geometry added, I’ll add tangent constraints to each line… To finish up, I’ll add a dimensions for the circular profiles… And the sketch is fully constrained. I’ll extrude these profiles as a solid, to a blind depth of twenty five millimeters.
With the base extruded, I’ll go ahead and hide the default reference planes from the workspace... Next, I’d like to add a draft to taper the profile and give it the overall shape I want…. I’ll click the “Draft” icon and select the bottom face as the neutral plane… then select any side as the “entities to draft”. Because “Tangent Propagation” is enabled, only one side of the profile is required for this selection. I’ll enter fifteen degrees as the draft angle… make sure that the draft is applied in the direction I want… and click OK.
With the base for this device complete, I’d like to add a sphere for the round ball joint at the tapered end.
<Sketch requires converted entities on top and bottom, draw line on left face (connect endpoints), find center point of upper line, create 2 lines with endpoint at center-point of upper horizontal line, make lines parallel to far left line and then create 3 point arc intersecting upper left endpoint, create a construction line overlapping the two lines for revolve axis>
To create the sphere for the ball joint, I’ll start a new sketch on the right plane and look normal to the sketch plane... Before starting the sketch, I’d like to convert some of the existing geometry so I’ll just right click and select “use” on the geometry I’d like to convert. With this geometry shown, I can use the end-points to locate geometry for the ball joint sketch.
I’ll sketch a line parallel to the drafted face of the base… then I’ll add a three-point arc that will intersect the end-point of this line…. I’ll give the arc a radius dimension of thirty one millimeters... and to finish up, I’ll add a construction line to position this arc and fully constrain the sketch….and convert an existing line to construction….
With the sketch complete, I’ll select the icon for the “Revolve” tool… And pick the closed profile just created… I’ll make sure to select “Add” to merge the sphere into the base … And for the revolve axis I’ll select this construction line. For the revolve type, I’ll be sure to select “Full” to make sure a closed sphere is created and I’ll merge this feature into the existing part. I’ll click OK to finish the Revolve.
At this point I’d like to create the lower section of the part.
Because I want this part to have symmetry, I’ll create this sketch on the right plane that bisects the part, and I’ll use mid-plane extrudes to maintain the symmetry.
To save a little bit of time here, I’ll skip ahead to a finished sketch with three closed profiles…. and I’ll click the icon for Extrude. I’ll select the interior profile first and make sure to choose ”Add”… I’ll change the End Type to “Symmetric” at a depth of thirteen millimeters… I’ll click OK and the new geometry is added.
To finish this profile, I’d like to taper the shape, to do this I’ll again use the Draft tool. I’ll select the base as the neutral plane and select both flat sides of the geometry as the Entities to Draft, and set the draft angle to three degrees. I’ll click OK to finish.
Now that one of the sketched profiles has been extruded, the sketch has been hidden. I’d like to use the two other profiles for this next extrude, to do this I’ll show the sketch once again from the features list…. And extrude these profiles to a symmetric depth of three millimeters.
With the basic shape of the part now created, I’d like to add a few more details to the design by adding some through holes, and then filleting the edges to break all of the sharp corners. I’ll create another sketch on the Right plane for the through holes I’d like to add.
For this sketch, I’ll create a couple of circles and offset existing geometry to create the boundary for the through holes…
I’ll skip ahead once again to add a bit more detail to the sketch for the holes… and before I use the extrude command create the holes, I’ll add a couple of sketch fillets to create a smooth opening for the holes. At this point, I’ll once again select the icon for “Extrude”.
I’ll make sure to enable the “Remove” option this time, and for the “End type”, I’ll choose “Symmetric” and enter a depth of thirty eight millimeters to make sure that all of the material, in both directions is removed.
To finish up the part, I’ll add a few fillets. Keep in mind that since there are some areas where fillets will overlap with one another, multiple fillet features are required here. I’ll be sure to place fillets on all of the sharp angles of this part.
With the fillets added, I’ll give this part a name…. and the part is complete.
Before wrapping up, I’ll open an assembly tab that includes this part and a socket mockup. This part has been set to “fixed” in this assembly and I’d like to mate the part created earlier to test movement similar to a hip joint. To do this, I just need to add a single mate to this assembly. I’ll select the “Ball mate” from the toolbar… and select each of the corresponding mate connectors. I’ll click OK, and with this mate added the assembly is complete.
To test out the functionality of this assembly, I’ll select the Ball Joint part and then use the drag manipulators here to test the range of motion. And as you can see, this ball joint performs just like you’d expect.
Introduction to Assemblies and Subassemblies
Working with assemblies in Onshape allows part studios to come to life, enabling motion and degrees of freedom between parts. Assemblies combine parts from part studios into a single workspace, where parts can be constrained relative to one another using mates. Assemblies can be created using either a bottom-up approach or an in-context approach. A bottom-up approach combines individual parts that were created in separate part studio tabs. These parts have no relations to any other parts until they are inserted into the assembly. Assemblies can also be created using an in-context approach, which means all of the parts that will be added to the assembly are created in-context in a single part studio. This method ensures that all of the components will fit properly in the assembly. Subassemblies can also be created, which is when one assembly is inserted into another assembly. Let’s take a look at an example in Onshape that demonstrates these assembly design concepts.
When multiple parts are created in a single part studio, they are rigid and cannot move relative to one another. When those parts are brought into an assembly…..all of their constraints are released and can move separately from one another. …..
To add constraints back to the parts, mates are used to restrict certain degrees of freedom so that parts can move relative to one another as intended in the design. ….. Unlike part studios, when a subassembly is inserted into another assembly, it retains all of the constraints that were added to it.
When creating assemblies in Onshape, there are two primary approaches that can be taken: the bottom-up approach and the in-context approach. The bottom-up approach takes individual components from separate part studios and adds them into an assembly. This approach is commonly used when adding off-the-shelf part models or imported part models into an Onshape document. Here there are a number of individual part studios shown at the bottom, each containing a single part that is used to create a bottom-up assembly. If I activate the “Bottom-Up Subassembly” tab…..you can see that three of these individual parts were added and constrained in the assembly…..the wheel, multiple instances of a spacer rod, and a wheel without a cutout. Each of these is fully constrained relative to one another, but if I suppress the last mate feature in the features list…..I can move the wheel without the cutout away from the rest of the model. …..
Now if I activate the “Bottom-Up Assembly” tab…..you can see the subassembly listed in the features list along with the individual mount and crank parts. If I suppress the two mates in the features list…..the individual components and the subassembly can be separated from one another. …..
However if I unsuppress the mate features…..
all of the constraints are reapplied. Now the assembly is free to move with the mates constraining their respective degrees of freedom.
As opposed to the bottom-up approach, the in-context approach has the user design all of the parts in a single part studio and then insert them into an assembly. This guarantees that the part geometry will fit in the assembly just as it fits in the part studio. This approach is great for creating models that have specific mechanical functions and geometric constraints. The “In-Context” part studio in this document shows all of the parts created in-context to one another. Because these parts all fit together in this part studio, I know that they can be mated in such a way that all of the parts will fit geometrically in the assembly. This is not necessarily the case when using the Bottom-Up approach. If I switch over to the “In-Context Assembly” tab…..notice that there are no subassemblies appearing in the features list.
This is because all of the parts were mated directly here in the assembly. When using the in-context approach, entire part studios can be inserted into the assembly. ….. Even though all of these parts are free to move in the assembly, they are positioned exactly as found in the part studio. This means that if any components are positioned properly relative to one another and do not need to move, they can be grouped together. ….. I’ll select all of the components that make up the wheel subassembly as shown earlier…..and use the “group” mate to group them together and constrain them relative to one another. ….. Now these parts will move together as a group. …..
Adding a couple other mates will complete this assembly. I won’t go into too much detail here about the different mate types since they are covered in another video. First I’ll make sure to “fix” the mount in place so that it doesn’t move when adding mates…..and then I’ll add a “revolute” mate to allow the crank to spin freely inside the mount. Adding this mate constrains five degrees of freedom, allowing the part to rotate about only a single axis. The icon for each mate type also helps visualize how the components will move once the mate is applied. ….. Now all I have to add is a “fastened” mate between the wheel and the crank. This mate constrains all six degrees of freedom, as if the two parts were glued together. ….. Now the parts are properly constrained, and the crank spins the wheel about the mount.
When creating models in Onshape, it is important to understand if a bottom-up approach or an in-context approach will be best for creating an assembly. While inserting entire part studios streamlines the assembly process, a bottom-up approach may be necessary when dealing with off-the-shelf or imported parts. Nonetheless, both methods work well to create assemblies that can move and simulate realistic mechanics.
Documents in Onshape enable you to work with parts, assemblies, and drawings all within a single workspace, and that combined with the multipart functionality in part studios opens the door to a wide variety of design techniques and workflows. Let’s take a look at a quick example using some top-down and bottom-up design techniques, all within this single document.
A new Onshape document contains a part studio tab and an assembly tab, and as you may expect, you can create as many tabs as you need. The workflow in Onshape is simple. You create all of your geometry within part studios, and when you’re ready to add motion, or bring parts or sub-assemblies together from other tabs, you do so in an assembly.
A part studio can contain as many parts as you’d like it to; in other words, You’re not limited to a single part per part studio.
This lets you easily design additional components and create the in-context relationships between them. For instance, I can start a new sketch on this face. I’ll select these four circular edges and click the “use” icon to convert them into sketch geometry.
Next, I’ll sketch some lines to connect them, and trim away the unnecessary geometry. For the sake of time, I won’t bother fully defining this sketch….. I just want to create the rough shape I’ll need, and can come back to add dimensions later.
Once I have the profile roughed in, I’ll create the extrude feature. I’ll choose the “New” option so that this extrude will result in a new part. I’ll extrude this a quarter of an inch. Once the preview looks the way I want, I’ll click the check, and the new part is created and added to the tree.
Let me quickly give this part a more descriptive name. I’ll right click the part in the tree, and select rename. I’ll change the name to Bracket and click the green check.
You can continue creating as many additional parts as you need. For Instance, I can mirror this part about front plane. This multipart workflow is intuitive and expected in Onshape.
Next, I’ll switch over to the assembly tab, and insert these parts into it. I’ll click the insert parts and assemblies icon, and select the entire part studio. When I click the check, the parts are inserted. While in the part studio, these parts were more or less fixed relative to one another, but now that they’re in an assembly, I can simply click and drag them to move them if I’d like. I’ll click undo. I could now add mates to create motion between the parts, but instead, I’d like to keep these grouped together as is, so I’ll select them all, and click the group icon. When I click and drag them, they move as a unit.
As I mentioned earlier, assemblies are also used to bring items from separate tabs together.
This damper model was designed by a colleague in its own part studio…..and if I switch over to this other tab here…
you can see there’s a damper sub-assembly, created as well. This already has some group and slider mates added to control the motion of the piston. So not only can you insert multiple part studios into the main assembly, but you can work with subassemblies if you’d like, as well.
I’ll go back to the main assembly, click the insert icon, select assemblies, and insert this damper sub assembly. I can add a revolute mate to join it to the linkage parts.
As you would expect, any changes I make to items in their part studios will propagate here to the assembly. I can go into the linkage part studio for the bracket I added a few moments ago, ……roll back before the mirror and create a fillet on the outside face……Then I’ll roll forward to the end….. and when I switch back to the assembly tab, you can see the fillets added there, too.
Onshape also allows you to upload any type of file you can imagine into a document, which is useful since a typical project can often require a large collection of documents……ranging from marketing materials,……manufacturing specifications……..supplier quotes, and so on. You can store and work on those files within this single document.
I have a SolidWorks part file for a fastener that was provided to me by a supplier.
I’ll add click the plus sign to add a new tab to this document, and click Upload. I’ll browse for the file and upload it and you can see a new tab is added right here at the bottom. I’ll translate the fastener into an Onshape part studio…. And then insert two instances into the assembly. From here I could go on adding mates to position them.
The single document concept in Onshape lets you easily switch between using a bottom up assembly design approach like this,
You accomplish all of your modeling and designing in the part studio environment, and then when you’re ready to bring things together from other tabs or add motion and interaction between your parts, you can then bring them into the assembly and create the appropriate mates. Onshape makes it very intuitive, whether you’re using top down methods with a multipart workflow, bottom up methods by combining separate part studios together in an assembly, or importing cad files from other traditional systems.
Let’s take a look at adding mates to your assemblies in Onshape. I’ll go ahead and switch over to this empty assembly tab….and insert everything from the part studio. When I do, all of the parts are completely free to move and have all their degrees of freedom. To get started I would first like to Fix one of the parts so that it removes all of its degrees of freedom so all of the other parts can be mated with respect to it. To do this I can simply right click on any part in the graphics area…or features list and select “fix”. Any part that is fixed will have this icon next to it in the features list. I can of course unfix it by right clicking on it again, but I’ll leave it fixed for now.
Onshape defines mates based on the intended behavior that you would like as a result, such as fastened, revolute, slider, planar, cylindrical, pin-slot, and ball.
For the first mate I would like to add, I would like to have this part …slide along the base….so I’ll choose the slider mate icon. When I do, you can see Onshape is prompting me to select what are known as mate connectors, which are at the heart of adding mates in Onshape. If I roll my pointer over any face….you can see small dots appear. These dots are locations on faces where you can establish mate connectors. If I roll over one of these dots, notice a small triad appears. What’s powerful about mate connectors is that, they are not just locations on faces or edges, but rather actual coordinate systems with their own X, Y, and Z axeez, and the orientation of the axees is important to take note of, particularly for certain types of mates like this slider mate I am adding here. A slider mate will allow two mate points to slide along the blue, Z axis of the triad.
If I wanted to use this connector location here, notice as I wake up the different faces and roll over the preview of the mate connector, the triad is oriented differently. Alternatively, if I wake up this edge, and roll over the mate connector, you can see the triad is oriented with the Z axis, normal to the edge. I’ll go ahead and select it with the triad in this orientation. For the second mate connector, I can roll over faces of the other part, and the same principle applies here as well. I want to pay attention to the orientation of the triad, in this case using with the edge or the face. When I select it, the part snaps into place. Notice there are icons to flip the primary….and secondary axes….in case you need to make any adjustments to get the result you’re looking for. And when I click OK, you can see the part is now able to slide along the other.
Also, in the features list you can see the slider mate listed here. If I double click on it, notice the drop-down allows you to change this to any of the other mate types, or even re-define any of the mate connectors in case you do need to make adjustments or use a different orientation for the mate connectors. I’ll go ahead and close this. So with this single mate added using mate connectors, I was able to remove several degrees of freedom in a single step to get the behavior I was looking for. Let’s continue on and add mates to the other parts.
For this next one I would like to fasten the spindle inside the shaft. The “fastened” mate type removes all degrees of freedom between any two mate connectors, so they are essentially glued together. For the mate connectors, I’ll select the point on the face inside the shaft….and on the face of the spindle. Again I can use the flip axes buttons.
At this point, if I rotate one of the parts….you can see they both rotate together.
Next I’d like to mate this with the sliding jaw. Looking at the toolbar you can see there are options for revolute and cylindrical. Revolute removes an additional degree of freedom than cylindrical, but rather than explaining, let’s just take a look. I’ll select cylindrical for now. For the first mate point, if I roll over the cylindrical face of the jaw, you can see there are three default mate connector locations along its axis. Alternatively I could roll over the back face and use the point here. As a side note, if you ever find yourself having trouble selecting a particular mate connector, due to other faces being woken up by your pointer as you move it, one thing to note is that you can hold down the shift key on the keyboard to keep the mate connectors showing on the screen as you move the pointer.
I’ll select this point at the rear of the cylinder…and repeat the process for the shaft. When the parts snap into position, you may notice that previous mates that you have added are not solved during the step of adding the new mate, and in instances like this you can click the solve button. Again, if needed you can click the flip axes buttons. And I’ll click the green check to finish.
At this point when I move the spindle, you can see it is free to rotate about the mate connector, but of course it is also free to move along the axis as well. This is due to the cylindrical mate type I defined it as. Instead, I’ll double click the mate….change it to revolute….and click the green check. Now when I move the spindle, you can see how the revolute mate allows the spindle to rotate without moving away from the mate point on the jaw.
One last thing. In this example, I used the mate tools on the toolbar to select mate connectors as I was creating them, but keep in mind, you can always use the mate connector tool to precisely define the location and orientation of mate points ahead of time. You can even add mate connectors in your part studios and they will be available when you bring parts into an assembly.
Mates and mate connectors are powerful, and as you can see here, only three mates were added to get the behavior I was looking for here in this example. As you get started using mates in Onshape, I recommend playing around with the different mate types and the effects of using different mate connector orientations and you will quickly see how mates can make your assemblies come together efficiently as well.
Assembly Design Case Study
Let’s get some practice working with assemblies here in Onshape. In this exercise I’ll create a new assembly studio with these components and talk you through the mates I’ll be using to assemble them.
To get started, I’ll add a new Assembly Studio here in this document……and I’ll go ahead and click the “Insert” icon on the toolbar. I’ll go ahead and click on the entire Part studio to insert all of the parts contained within it here in this assembly. To get a better idea of what we have here, I’ll just spread some of the parts out so you can see them all.
<Fixed & Fastened Calipers>
Typically, when I start a new assembly I like to “fix” one of the parts in 3d space so it can’t move around when adding mates with other parts. I’ll right click on the Inner Caliper part and Fix that one. First, let’s go ahead and take care of mating the outer caliper, and I’ll come back to the rest of the components.
A simple approach for this one is to fasten it to the Inner caliper between two mate connectors, so I’ll select the fasten-mate icon. Since both of these parts were designed within the same part studio with a tight relationship between each other’s’ geometry, there are quite a few features between these parts where a single mate connector will position and orient them perfectly.
I’ll roll over this face of the outer caliper….and anytime I select a mate point it’s helpful to take note of the orientation of red green and blue axees of the triad. In the case of a fastened mate, the orientation doesn’t matter a whole lot since it is removing all degrees of freedom between mate connectors, but for other mate types that leave degrees of freedom the orientation of the triad lets you know how those types of mates will behave once they’re applied.
I’ll select the mate connector……..and repeat the process on the other caliper. When I do, the parts snap together. So at this point the two calipers are mated together and cannot move anywhere because of the Inner caliper being fixed, and outer caliper being fastened to it.
<Revolute Mates for Hardware>
With the inner and outer calipers mated together, let’s work on mating some of the hardware. It’s common to have situations where several of the available mate types will accomplish what you’re looking for, but it’s up to you to decide which behavior you would like. For instance, I could simply use a Fastened-Mate to connect the mate connector at the center of the hole….with the connector at the center of the round face on the bolt.
So this work here, but cylindrical or even revolute might be good choices as well. The icons representing each mate type are helpful for understanding the resulting degrees of freedom. Here you can see “Revolute” allows a degree of freedom to exist for the part to rotate about the blue axis of the mate connector triad, but no other degrees of freedom. I’ll go ahead and select it….and flip the orientation….and you can see the bolt can only rotate about the hole.
I’ll repeat this process for the guide pin…..again using a revolute mate type, but a fastened mate type would work fine here as well.
For the bleeder screw, I’ll go ahead and use a fastened mate to remove all of its degres of freedom when I mate it to the caliper.
<Insert Additional Components or Copy-Paste>
When I created this assembly studio, I inserted all of the parts that were in the part studio, but notice in the part studio there was only one instance of each component. To add additional instances here in the assembly, I can click the Insert icon….and just select it from the part studio….but in some cases it may be faster or easier just to copy a part directly from the assembly studio your working in. To do this just right select the part you would like to copy…select copy….click in white space to deselect, and then I can either press control-V on the keyboard, or if I right-click you can see I can paste the part from here.
<Insert bolt part from insert menu and copy/paste the guide>
For the sake of time I’ll skip ahead for a moment and go ahead and mate these items using the same mate types I showed you a moment ago.
<Cylindrical and/or Slider Mate for Piston>
Next, let’s turn our attention to mating some of the internal components of the assembly. To make my selections easier, I’ll go ahead and hide the Outer Caliper.
Starting with the piston, I have a couple of options for mating it to the bore in the caliper. The cylindrical mate type provides a behavior that allows rotation and translation about the blue axis of the mate connector….but in this case, the piston doesn’t really need to rotate about the axis, but it does need to translate, so the slider mate type will also work here. I’ll go ahead and select it….but keep in mind you can always just change the mate type after it’s added in case you would like to change its behavior.
For the mate connector I can roll over the cylindrical face….and hold down the shift key to key the mate connectors on the screen as I roll over them…..paying attention to the orientation of the blue axis. Or, if I let go of the shift key….and roll over the flat circular face, the triad appears in the same orientation. On the caliper, I can again either use a mate connector from one of the circular faces, or the cylindrical face…..and it snaps into position….so I’ll click OK.
For the seal, I’d like to just fasten that to the piston, removing all of its degrees of freedom. For the connector, I’ll roll over this outermost edge so the connector will be positioned at the extent of the part…and hold down the shift key to select it. I’ll roll over the piston…and select this connector as well. At this point if I click and drag the piston, you can see it can slide along the hole in the bore with the seal.
<Planar Mate for Brake Pad>
For the brake pad I’ll use a couple of mates to position it with respect to the guide pins and the piston. The behavior I am looking for is to have the pad slide along the guide pins, and to have the back face of the pad stay connected to the piston. I’ll start with the guides.
I’ll select a slider mate type….and for the connector I can use a location from the circular edge….or cylindrical face of the pad…..and repeat the process on the guide.
When I move the pad you can see this gets the desired behavior of sliding, but it is still able to rotate….so I’ll go ahead and add another slider mate with the other guide… and flip the orientation.
To keep the piston in contact with the brake pad, let’s see what happens if I try to add a fastened mate to connect them. When I roll over the second mate point, the problem here is that these two mate connectors are not aligned, based on the position of the parts from the previous mates, but I’ll go ahead and click OK anyway. When I do, the parts snap into position, but several of the previous mates change color in the features list, letting me know there is a conflict.
You can always click undo, or press control-Z to undo. Since the mate connectors I selected were not aligned on the faces I selected, a better option that will work here is the planar mate, so I’ll select it, and click OK. When I do, you can see the parts shifted slightly in the graphics area, and the mates in the features list are all resolved.
I’ll go ahead and show the outer caliper.
<Pin-Slot Mate for lower bolt>
Let’s add the bolts that will go into these slot shaped holes. I’ll select one of the bolts to copy it…and I’ll paste a couple of instances of it. While I could add a cylindrical or revolute mate to one of the circular areas of the slot, that would not allow the bolt to translate within the slot. The pin-slot mate type is perfect for situations like this.
For the first mate connector I’ll roll over one of the cylindrical faces. It’s not important whether I select the left or the right cylindrical face since there will be a degree of freedom from left to right anyway, but I do want to select the mate point that’s planar with the face of the caliper since that will determine position of the bolt relative to the face. Take note of the orientation of the triad…I’ll do the same with the cylindrical face of the bolt.
I’ll click OK….and you can see the bolt is able to move within the slot.
For the sake of time, I’ll skip ahead and repeat the process for the bolt in the other slot.
<Ball Mate for the Maintenance Bleeder hose>
Here in this assembly I have an item representing a maintenance hose that would connect to one of the bleeder valves. For this item I would just like to show how the part would be connected and be able to position it anywhere with it being connected to the bleeder.
The ball mate allows you to attach two mate connecters together while retaining all of their degrees of freedom.
For the first mate connector I’ll select the inner face of the round section of the bleeder….and for the tube, I’ll roll over the outer flat face to use the mate connector. I can of course flip the orientation but in the case of the ball mate, the orientation doesn’t matter a whole lot since all degrees of freedom are retained anyway. When I click OK….you can see how the hose is able to move freely about the bleeder.
<Mate Connectors in Parts>
Throughout this exercise I have assembled each of the parts in this assembly by leveraging the default mate connectors that showed up when rolling over each face, edge, or vertex. There will of course be situations where you want to position something in a spot where you might not have a default mate connector. In situations like this you can add mate connectors in the part studio to use for adding the actual mates in the assembly.
I’d like to position this part in a specific spot here on the caliper. Let me switch over to the part studio for the caliper. Before clicking the mate connector icon, I’ll want to sketch a reference for positioning the connector. I’ll just use a sketch point….and make it vertical above the origin….I’ll give it a dimension….and exit the sketch.
I’ll click the mate connector icon….and for the origin entity I’ll select the sketch point….and for the owner part, I’ll select the caliper. Just as when adding mates in an assembly, the orientation of this mate connector is important.
I would like the blue axis to be perpendicular to the circular face, so I’ll click “realign”….and for the primary axis I’ll select an edge that orients the blue axis….and you can always use the flip axis icon if necessary. I’ll click OK, and the mate connector is added. When I switch back to the assembly studio….you can see the mate connector is available for adding the mate.
For this I’ll use a fastened mate….and select the default mate connector on the part…..and the mate connector I added a moment ago to finish up.
Edit History & Versioning
As you work in Onshape, everything you create or modify in your designs is saved at all times. If I change a couple of dimensions here, I don’t have to worry about saving any changes here in the document. In fact, if you take a look at the toolbar, notice there is no save icon. Anytime you close your browser, or even in case you were to lose your internet connection, you can be sure that the latest changes are stored in your Onshape document.
One nice thing about Onshape perpetually storing everything you do, is that you essentially have unlimited undo capabilities. If I click undo here on the toolbar….I can undo the changes I made here in this browser session….
In a previous browser session I had modified the height of the base here in this design.
If I roll over this icon here….notice there is also “Workspace History “. Workspace History allows you to roll back to view and-or restore any changes that you have made, all the way back to the initial creation of the document, regardless of what browser session they were done.
You can view the state of the design at any point in its history by just clicking on it here in the workspace history. If you would like to restore the main workspace back to this point, you can do so by expanding the gear icon and clicking restore…..or just click “restore” at the top.
In addition to the perpetual save and unlimited undo capabilities in Onshape, you also have the ability to save versions of the design at any time. You can think of versions like taking a snapshot of the design in its current state, which of course you can come back to later as well.
If I roll over the “Manage Versions” icon….and click it….here I can save a new version of this document, and as a side note, this version will store everything contained in the document including any and all part, assembly, or drawing studios you might have in it. When I click it, a dialogue appears where I can enter a version name…..and a description. I’ll go ahead and click save….and the version is added.
If you take a look here next to the document name, notice the word “main” here. “Main” refers to the active workspace that I have here on the screen. As you work in Onshape, you can always think of main, as a working copy of the document. Any versions that you save, you can think of like snapshots of the design at a previous point in time.
If I again click the manage-version icon, I can see all versions of the document that have been created. and if you look at the top, here you can see “main” listed, as well as previous versions of the design that have been stored, including the one I created a moment ago.
Versioning not only provides a method of managing revision, but also provides a powerful method to collaborate on designs, which will cover in depth in another video.
Collaboration (Simultaneous Editing and Branch Editing)
Collaboration is a hallmark of Onshape, and is unrivaled by any CAD system on the market today. Onshape provides simultaneous editing capabilities within the same document, as well as a powerful concept of branching editing, allowing designers to go off into their own workspace to work on the design, or perhaps develop alternative concepts, and then merge changes into any version of the design.
Let’s start by looking at Simultaneous Editing. What I mean by “Simultaneous Editing” is that any number of people can open and work on the same document at the same time. To demonstrate here in this video, I’ll just create another instance of Onshape running here in my browser but keep in mind what I’m about to show you will behave the same way whether you have two people or twenty people working in the same document from their own devices or browsers. Let me show the two browsers side by side so you can get a better look.
When another person opens the document you will see their initial appear, as well as in the part studio they are looking at. You will also see their initial in any sketch or feature that they are editing.
As soon as one person makes a design change….everything is updated in real-time without the need to rebuild or reload the document.
To take this a step further, let’s take a look at when two designers are editing the same sketch. When I do you can see the initial on both screens editing the same sketch. Here on one screen, as one designer adds geometry….you can see it appears right away in both windows. Of course, this works both ways, and either designer can make edits, or add additional geometry and both see the same thing in real-time.
I’ll go ahead and exit out of the sketch in one of the browsers here…..and when I add a feature based from this sketch…..when I complete the feature, as you might expect, both screens update in real-time.
Simultaneous Editing is obviously powerful, but as I mentioned earlier, another innovation in onshape is something called Branch Editing, where designers can create a workspace based on an existing version of the design, make any additions or changes, and then merge changes back in with any version. Let’s take a look.
If you take a look next to the document name, you can see that both of these are working on the version called “main”. To branch off of a design, it must be based on an existing version. That said, let me go ahead and save a new version of the design with the changes that were just made.
The version was saved, but again you can see that both screens are working on the main workspace. Here in this tree view, I can see all of the versions that have been stored up to this point. If I expand the gear icon, here you can see the option to “branch to create workspace”. As a quick side note, if I click the gear icon for “main”, notice that option does not appear. This is because a branch must always be created from an existing saved version, or in other words since “main” is considered a workspace that may always be changing, a branch must be created based on a version that was stored which will not change. I’ll go ahead and create a branch from the latest version….and here in the dialogue I can type in a name….and a description.
When I click “create”….here you can see the branch has been added, and the white dot lets me know that this is an active workspace that I can click on to open, just as I could with main. When I open it….notice its name appears next to the document name, while “main” appears next to the document name in the other browser.
I can go ahead make some edits here in this workspace, and of course any changes I make are being stored in real-time within this workspace, where any number of designers can work as well.
Now keep in mind, in this other session that’s working with the main version, changes to the design can of course be made here as well….
So here I have two sessions where changes have been made to two different workspaces in the document. To merge them together, I’ll again click the manage versions icon ….
Something nice about merging, is that anything can be merged together. What I mean is, I can merge the change that was made in “Main” into the New Workspace, or merge the change that I made in the new workspace into the main workspace.
I’ll select the workspace I want to merge into, and click Merge. When I do, the “merge from” dialogue appears. Since I selected Merge on the new workspace, you can think of this like merging the changes from main into this workspace. I’ll click cancel…..and this time I’ll select the main workspace ….and select merge. By doing this, I can merge the changes from the new workspace into the main workspace, which the other session is already working in. When I click OK….right away you can see the other browser update, showing all of the changes merged together in the main workspace.
At this point either designer could continue working on any branch or workspace within the document as they wish. Branch Editing is not limited to a simple example like the one I showed you here. From any branch, you can save new versions, branch out even further, and merge changes from any branch at any time…and as you can see in this example here, branch editing really allows for powerful and flexible collaboration in Onshape.
Working with Existing CAD Files
Whether you’re migrating data from a traditional CAD package into Onshape, or working with a partner using one of the many different computer aided design systems on the market today, Onshape recognizes the value of your existing data and the value of collaborating with others, even if they are using other CAD platforms. Onshape allows you to import any type of file you can imagine into a document. Here, I’d like to focus specifically on CAD data. Onshape allows you to bring in Parasolid, Sat, Step, and Iges files, as well as native part files from Catia V5 and SolidWorks. For assemblies, Onshape can read in parasolid and step files.
Let’s say you’re working with a supplier who’s using a traditional CAD system, and they provide you with a CAD file, but you need to make some modifications to their design to fit the needs of the project you’re working on.
In this example, a supplier sent me a SolidWorks file. Right here in the documents list, I can click the icon to upload a file…….. Browse for the file I need, and click open….and then OK. This creates a new Onshape document containing the file translated into an onshape part studio, as well as a tab containing the original uploaded file in case I’d like to share it, add properties to it, or redownload the original again later.
<Note: File will be in a “Supplier Parts” folder in the actual video and not on the desktop with other icons……>
So, when I uploaded the SolidWorks file, Onshape created this new document, but in case you already have a document that you’re working with where you would like to bring in the model, you can click on the plus sign in the lower left hand corner, and select “Upload.” I’ll browse for the file I’d like to upload, and click “Open.” The file uploads, and in just a few seconds you can see a new tab for the uploaded file in this document. I can click the tab to reveal properties of the uploaded file. Since this is a CAD file I may need to modify, I can also translate it into an Onshape part studio by right clicking the tab and selecting “Translate.” Keep in mind, you don’t necessarily have to translate the file, but if you want to take advantage of Onshape’s modelling tools, you have to first translate the file into an Onshape part studio. For the format, I’ll select “Onshape.” If this were an assembly file, I could choose to flatten the assembly into a single part studio, but since this particular file is a single part, I’ll just click OK, and the part is translated. I’ll click on the newly translated part studio tab, and you can see the geometry. There’s also an Import feature in the features list.
I need to make a few modifications, and since this imported geometry does not have any feature history I can take advantage of Onshape’s direct editing tools. I’ll use the move face tool and translate these two faces by a half inch using this edge for the direction to thicken them up for increased support.
I’ll also quickly add a couple fillets to these circular edges.
Now that I was able to quickly make that design change, I need to send the updated file back to the supplier. All you have to do is click “Share”, and anyone can access this file directly here in Onshape, from any device or any browser.
As a side note, I can translate the part studio to a Parasolid, sat, step, iges or catia file, and then download the translated model. To do this I can right-click on the part studio tab, and select translate….Or I can export it to an STL if I wanted to 3D print it. I’ll select Translate…..and I’ll translate it to a parasolid……..
When I do, this creates a new tab for the parasolid here in the document. Then I’ll right click the tab for the newly created parasolid and click Download.
And here I have a file ready to be imported into a multitude of other 3D cad systems.
Introduction to CADlessons beginner