who do I group a set of scketch entities

no_name433

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

SethF

A link to a publicly shared document would go a long way for people to troubleshoot your specific situation, but I think you're having a very similar issue to this post here. Your sketch has to be fully defined in its own reference frame. 

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.

wayne_sauder

@no_name433
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. 

eric_pesty

You can also select the group of things you want to move without fully constraining them using the transform command, this will let you move them all at once (but the result won't be "parametric", ie the position will not update later on). You can move the manipulator origin to existing reference point (you may need to add one if you dont' already have it) and when you drag this point will snap to other geometry. 

angelo_scozzarella

Is there a way to full constraint a sketch with a single command?

S1mon

Drag select all, use the Fix constraint.

angelo_scozzarella

Thank you.

Curt_Welch

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?

S1mon

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.

Design_Bro

https://forum.onshape.com/discussion/comment/108929#Comment_108929

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.

rick_randall

Like eric_pesty said - the transform command performs this function on sketch entities just fine, as is.

Design_Bro

https://forum.onshape.com/discussion/comment/119218#Comment_119218

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.

eric_pesty

https://forum.onshape.com/discussion/comment/119220#Comment_119220

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).

Design_Bro

https://forum.onshape.com/discussion/comment/119224#Comment_119224

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.

glen_dewsbury

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