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How can I resize a large number of sketch entities without changing their location?
alex_goldman057
Member Posts: 1 ✭
I am working on a part studio where multiple parts with linear patterns of holes need to overlap so the holes maintain their concentric relationships. I have done this by taking the original sketch with my hole pattern and copy/pasting it into other sketches from which I am extruding the various parts. I assumed that the linear pattern constraint would survive copy/paste so that, in the sketch where I need the holes to be smaller but still on the same hole pattern, I could just resize the hole that the pattern is based on, but the problem is the initial sketch with the desired hole pattern is a shape with the correct hole pattern that is then repeated with another linear pattern (a pattern within a pattern). I have since had to release that pattern to make adjustments, so the enveloping shapes are still multiples, but no longer constrained by a pattern, even though they have holes that are placed according to a specific pattern. All that is to say, I now have something like 200 holes that I want to resize. Is there a tool I can use to resize all of them at once without changing their locations? Either in the sketch or in their resulting parts?
Thanks in advance.
Comments
Use of the equals constraint on each circle in sketch might be helpful.
You most likely would be better off using feature patterns instead of sketch patterns. Sketch patterns can be very powerful and useful, but in most cases, if you can do it with a feature pattern, you probably should.
Here is a sample of linear pattern within linear patter using configurations. You can add more detail for hole spacing and calculated lengths and widths to suite your logic and needs.
https://cad.onshape.com/documents/dce3c5f6c9717f40901277de/w/fcaab14d969087547cdfbe2a/e/b77cfd81f97bc5294736fe72
I may have misunderstood the question, but could this be done with a variable?
This may be what glen is talking about.
My spidey sense is tingling when I hear about 200 holes in a sketch and overlapping slightly different sized holes too. The hole feature can create holes with a clearance and tapped hole in multiple parts in one go, then you can pattern it with a Linear Pattern feature. It will regenerate faster, and be easier to edit, and the holes will have the right metadata for the hole callout in drawings.
If you're already too far down your current path and just want a get-it-done bandaid you could resize the existing holes using the Move Face feature and could select them using the Create Selection dialogue. I made a video about it here. Ideally you'd go back and refactor the model to use a better approach, but these "bad practices" might get you to the finish line sooner than refactoring your model. I don't know your situation.
You can get better help here on the forum by sharing a link to your document assuming you're allowed to.
Independent Onshape Consultant | Industrial Designer
In the sample the variables are stored in the configuration table. You could put variables in the feature list but then you're back to copy and paste from part to part and loose the convenience of configurations. If you find an additional part is needed the just add to configuration list once the logic is worked out.
As Evan says, 400 holes to modify?? The feature patterns will give 400 holes and only the original instantiation from config table needs to be changed with a much better regen time.