Onshape Best Practices

I figured we should create a new thread for the response to the below post. If you have any suggestions, tips, or best practices for using Onshape, discuss them here.

Here’s our public CAD for reference.

  • We used one folder per subsystem (Drivetrain, elevator, ball tunnel, big beefy arm, etc)
  • We added an “Imports” folder in each folder to hold all the imported CAD files and reduce clutter
  • We tried to keep tabs for higher level assemblies to the left in the bottom bar, with sub assemblies to the right in descending hierarchical order.
  • We tried to make as few part studios as possible, with the goal being one part studio per subsystem.
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We use a very similar, if not identical, folder layout to what Ty described.

When designing in the Multi-Part-PartStudios we try to have the first sketch be the “master” driving sketch for the major components of the studio. The idea is to make it easy to modify a set of parts without having to find the right feature in the tree.

For example our elevator geometry is mostly all in the first sketch:
https://cad.onshape.com/documents/cc19b794ce1d39f2541c5749/w/efe96f2e13323d2ff40bd574/e/d8aba95b71709adc1e4c50a0

We learned late in the sason how to precisely position parts made with the Custom Length Extrusion FeatureScript. The trick being make a sketch on the plane where one end of the part needs to start and place a point in the sketch at the center of the extrusion.
If the extrusion needs to fit between two parts in a PartStudio you can make the extrusion undersized then use the Move Face tool to move “up to entity”.

We are also heavy users of the Lighten Feature Script to make the awesome cutout patterns with a CNC.

We found that many teams are making great use of the MKCad parts library however due to the many copies it can be challenging to link to the version that is kept up to date. We found that creating a label and adding just the original MKCad files to the label makes it much easier to find the desired part in the insert dialog:

We also learned the hard way that linking in parts and assemblies that change often from other documents was quite a nightmare. We use a single Onshape document for the whole robot and only parts that do not change (ex: Gearboxes, Motors…) are linked in from another document. The challenge of constantly updating parts from other documents wasn’t worth the potential benefits.

Here is our full robot:
https://cad.onshape.com/documents/cc19b794ce1d39f2541c5749/w/efe96f2e13323d2ff40bd574/e/8be591f8b7ffb665b67296b4

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Do you find that you have issues with long loading times on parts and assemblies that make heavy use of Lighten?

EDIT: Our Onshape organization and use is very similar to what’s been reported so far, including the use of tags to quickly find the MkCAD library.

We are careful when using lighten on a part to slowly select sketch regions and wait for the part to regenerate before selecting another.

As for loading time of an existing part that has been lightened, I haven’t noticed a significant difference between a lightened part and a similarly complex part constructed in a different manner.

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Can totally get behind the use of the lighten feature script we used it on some of our water jet sheet metal parts this year it makes the part have a very nice finished look and makes future edits very easy my only problem is its incompatibility with the sheet metal function can make it frustrating to work with at times