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In 2026, What Is the Best Sketch Blocks Workaround in Onshape?
Chris_Beckett
Member Posts: 15 ✭
I'm coming from SolidWorks and would like the same sketch blocks functionality in Onshape.
I've found a couple threads mentioning workarounds that are 3-5 years old.
Before I spend time trying them… what is actually the best workaround currently available in Onshape?
And is it on the roadmap to add sketch blocks functionality properly?
Previous thread found:
And this one:
Both were years ago. Any better methods now?
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Answers
It would help to understand what you are trying to do as there might be different workarounds depending on the application…
For logos, my preferred workflow is to create "zero offset" surface(s) and create a closed composite of that. I typically include a configuration variable to scale it to the desired size. Then you can derive it in at the desired size and extrude or whatever the faces of the composite. If the logo has a lot of separate elements, using a query variable might be worth it to use for an extrude. (and the "Query variable +" FS allows importing query variables so I would definitely do that going forward!)
If you are looking for moving things around at the conceptual level, you can create assemblies of sketches and use mates on these.
Here's an example:
Here are three examples how I've seen sketch blocks used.
Use Case #1: Logos
Just a 2D representation of a logo. Saved in our Design Library. Bring it into a drawing. Scale it up or down and reposition it to fit a title block. Or into a sketch on a part to make a cut or extrusion in the shape of that logo. You can position it and scale it as required. Without any other constraints. (The nature of being a block constrains it).
Use Case #2: Electrical Components
2D drawing of things like resistors. We sketch things like how to attach a resistor to a pcb, then reuse that same resistor sketch on all similar drawings. The sketch is in our library. Just grab it and go. It's almost instantaneous.
Use Case #3: Electrical Circuit Schematics
I sketched a circuit diagram in AutoCAD because it's more free form and very easy to copy, paste, and move things all around. Import that into a dummy drawing in SolidWorks. Copy the schematic from that drawing into my actual production drawing. Select all the circuit elements. Click "Make Block." Now I can drag and scale that schematic block anywhere on the drawing. This has been super helpful.
These are just a few but the principle applies to many other things. For example in SolidWorks there's a library of all common steel extrusion profiles. Just grab one, put it into your sketch and extrude. Couldn't be easier.
For the last issue, the Frame features and optionally custom frame profiles work beautifully.
Simon Gatrall | Product Development, Engineering, Design, Onshape | Ex- IDEO, PCH, Unagi, Carbon | LinkedIn
That's a great feature for weldments. Thanks for introducing me to weldments in Onshape (aka "Frames").
Although that is similar functionality to a sketch block, it's not the real use cases I'm actually dealing with. I just mentioned that as a similar example.
So for this particular thread, let's ignore that one. Though it does show that similar functionality is possible in Onshape!
Will keep trying things for my 3 main use cases.
Deriving a "surface" is a pretty decent workflow for this type of "bring in a shape you want to extrude" workflows, and once you get comfortable working with mate connectors (definitely something worth spending some time on as they are both a bit different and very useful in many places), it does give good control for positioning derived stuff.
For your other use-cases it looks like you are mainly talking about 2D drawings. Onshape's drawing sketching is still pretty limited, and doesn't let you "derive" things.
For a title-block logo, it might just be easier to use an image… Or you include that in a layout sketch of your title block (done in a part studio) that you dump in your drawing template as a DXF. Here's what that looks like for me (note the 3rd angle diagram in yellow that could be a logo):
I throw in a diagonal line in the sketch that locates things nicely in the drawing template (bottom left at zero, zero) and delete it after importing in the drawing.
For use-case 3, the Autocad import can just be in a sketch that you insert as a view in your drawing, you can scale and move it around just like any other drawing view so I would think this should work reasonably well.
For use-case2, I think it would be the same thing where you would just insert a "view" of your 2D representation into any drawing you need it, but it won't work well if you need to "connect" other other sketch elements together in your drawing.
Basically you won't be able to do much "2D" stuff directly in drawings in Onshape so you have to work with 2D elements in part studios and/or assemblies and just insert these "blocks" as views in your drawing.