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who do I group a set of scketch entities
no_name433
Member Posts: 3 EDU
Hi
I Am trying to copy/paste a group of sketch entities and then position the pasted entities in their new location.
I paste the group:
And then I am trying to coincide one of the points to a reference line so the new entities will be centered.
When I add the new constraint only one point moves to the new location, what I need is for the entire set of entities to reposition.
Is there a way of doing what I'm trying to do? What is the right way of doing that?
Thanks
Erez
I Am trying to copy/paste a group of sketch entities and then position the pasted entities in their new location.
I paste the group:
And then I am trying to coincide one of the points to a reference line so the new entities will be centered.
When I add the new constraint only one point moves to the new location, what I need is for the entire set of entities to reposition.
Is there a way of doing what I'm trying to do? What is the right way of doing that?
Thanks
Erez
0
Answers
Everything in this example the only dimension constraints are lengths of lines. When I had things defined with a point-to-point dimension to the spline control point, that dimension was not coming through, so I instead dimensioned the line to the spline control point instead. So from that limited experiment, I'd guess that certain ways of dimensioning and constraining may work better than others to make them able to copy and paste reliably.
I think it is an issue of not properly constraining the sketch entities. Make sure that your original sketch is completely constrained (ideally all lines and points turn black) then copy and paste. Yes, it is possible to do what you are trying.
So, the answer here is, "You can't do it." I also need to group a set of sketch entries for similar reasons as the original questions.
The sketch was a copy and paste from another document, but I want to parametrically attach this sketch to a reference of the part I've added it to.
The best I can do is fix all the entries, and use transform to move them. That gets it in the right place but there are no parametic updates when the reference point moves. It gives a constraint error instead. At least I know it's an issue, but then must remember later what it was attached to etc.
I can add 20 dimensions to the sketch to tie all the unconstrained entities together, but that's a pain worse than as justified.
What I want is a group command like in assemblies that lock the items to a group relative to each other but leaves the group still unconstrained. Then that group can be transformed to the correct location, and then hopefully move as the reference point moves.
Am I correct that this sort of sketch entity group feature just doesn't exist?
There's no built in group function like in other systems, but there are many ways to work around it. This is an older thread.
We can now use sketches like parts in assemblies if that helps. This can be good for 2D or even 3D motion studies.
Depending on what your sketch looks like you can also turn it into a surface in the part studio and then use the part transform feature to move, rotate or scale the surface. This can then be thickened or turned back into a sketch.
If the sketch "group"/"block" is something that you're going to use over and over, consider putting it in another part studio or even a different document and deriving it into other part studios to use it. In that case I would consider a surface or even part model approach to keep the derived geometry as a thing that can be placed and scaled however you want. I've done this for logos.
Bumping this. I'll look for or start an improvement request on this. But this would be very helpful for designers, since the text functionality in OnShape is quite limited; which forces us to bring in text as dxfs.
Like eric_pesty said - the transform command performs this function on sketch entities just fine, as is.
No, it doesn't. You are not able to parametrically move things this way unless you add relations to the entire dxf. Which, depending on what you're doing, can be quite a time-sink.
The workflow of adjusting a parametric sketch, then leaving that driving sketch to go to another sketch which has your dxf in it, then selecting all and transforming to meet the one line that did move is not what I'd call a clean implementation. It's a hack and is not conducive to product development.
It takes a 5 second adjustment to an equation or other driver, into a 30 second operation. Once you consider this is an operation you'll be repeating as you find your layout or other things adjust, it adds up to an annoying time-sink. While Solidworks did not have the most control over text, it could accomplish things like this fairly well.
There's a workaround if you are going to do this a lot: import your dxf with your text in a sketch, create a zero offset surface of all the faces and create a composite out of it.
Then you can derive this into your "design" part studio (either directly onto a reference mate connector, or you can use a transform feature to locate it).
Good idea, while it doesn't fix the issue it's a…useable enough Band-Aid for now. I should have thought of that since I use that for other things, thanks.
You could use the sheet metal form tool to punch where ever you like with out grouping sketchs then trying to make copies of the sketches. Once the form is created it is place able by many means. Individual sketches can use any sketch means needed including bring in DFXs to produce forms. If not sheet metal then just finish the s/m part.
https://cad.onshape.com/documents/27e55292bbcba38fdbd433b9/w/c71d872be347011a383a1fed/e/60856cbfccd149d735ff29b0
None of these workarounds do what we (I) actually want to do, which is to simple have a Group Constraint that behaves like the Group Mate. I want the sketch elements to move as one element in real time within a sketch, which we often use as a 2D kinematic workspace.
Maybe I misunderstood the original question, but I'll try a little more detailed explanation - (this is for a one time move, at the sketch level - and without parametric references)
This method will easily move the items in the original post, in a predictable manner,
Go to "transform sketch" in the help section and do a deep dive into what this command will do (they may do a better job of explaining this).
This particular command is one that I overlooked and underestimated at first. It is quite powerful when used correctly.
Hope this helps