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I made a dummy part to demonstrate the workflow I am intending to replicate. It is derived by a profile curve in one plane (say top view) and another profile curve in a different plane (say side view). Then project those 2 curves to make a composite (3D) curve. Then sweep a section profile along it.

My problem is the source drawing is coming in from a old school 2D format with everything (multiple views) on one sheet plane. So I can trace the profile curves from the 2D master sketch easy enough by convert entities. But how do I then copy/paste that sketch element onto a different plane in order to do above? I thought about making a block but that seems like a long way.

The 2d to 3d tools might work here:

This video can walk you through it.

I've actually never used the 2d to 3d tools, so they might be best, but it can be as easy as copy/paste. Open the sketch, copy the elements you are interested in, close the sketch, open a new sketch and paste. You will lose a bunch of constraints and it may not be in the orientation you want, which might make selecting the elements and creating a block a little easier to handle.

Thanks for that video. I was just blowing past the little sub panel that pops up after the 2D file loads, but turns out it has some useful utilities to specify & reorient sketch elements to preferred planes & reference those positions to develop 3D model. Easier than what I was doing manually.

Use a derived sketch?

https://help.solidworks.com/2022/Englis ... Redirect=1

Thanks for reminding me of derived sketch. I should use that function more in normal modelling. What I had not appreciated is that if I changed the dimensions of the base sketch, then all the derived sketches also get updated which is very useful. Its important to do the key selections in right sequence: select sketch, hold CTRL key, select destination face, then Insert > derived face. It preserves the dimension of the sketch itself, but it comes in as blue indicating you still need to align & dimension relative to the new face features in order to become fully defined.

What it doesn't do. I tried having 2 part models open simultaneously & tiling them. If I repeat above but select a destination face in a different model, the Derived Face function is greyed out. I guess that makes sense otherwise there would have to be some kind of behind the scenes link between the part files. So alternatively I have used the Ctrl-C (copy) & paste into new file sketch. But its totally flexible at that point so you have lock or redefine the sketch relationships.

Petertha wrote: ↑Wed Dec 04, 2024 1:32 pm What it doesn't do. I tried having 2 part models open simultaneously & tiling them. If I repeat above but select a destination face in a different model, the Derived Face function is greyed out. I guess that makes sense otherwise there would have to be some kind of behind the scenes link between the part files. So alternatively I have used the Ctrl-C (copy) & paste into new file sketch. But its totally flexible at that point so you have lock or redefine the sketch relationships.

No I suppose it won't allow you to derive a sketch from one part to another, but if they are in the same assembly, and you do it within the assembly, it will allow you to use derived sketch to place that sketch onto another part.

Sorry for duplicating one of my own posts, but this follow-up better belongs here.

Well I don't know what I was doing incorrectly before, but it turns out I can use Derived Sketch function to copy/transpose a sketch to any other plane, thus creating a new sketch. I was able to transpose to a part face but that's just an additional capability. When its first inserted to the target plane, the entities are all blue (undefined) because the group is not yet referenced to an origin point or whatever. However it does preserve the sketch entities between each other, kind of like a group. You can lock the sketch into a desired position by dimensioning or alignment. Where I was getting confused is the new sketch does not then turn black indicating fully defined. But I think that is SW way of saying its not, really. Because if the source sketch changes, then the derived sketch updates accordingly. Totally useful. This method saves some copy-paste clicking like I was doing before.

Actually it should change to black. I'd say you've just not defined the rotation. Put a constraint to make it parallel and it should go black (to check prior to this... grab and drag a point on the sketch entities and it'll rotate most likely).

Petertha wrote: ↑Wed Dec 11, 2024 11:46 am Sorry for duplicating one of my own posts, but this follow-up better belongs here.

Well I don't know what I was doing incorrectly before, but it turns out I can use Derived Sketch function to copy/transpose a sketch to any other plane, thus creating a new sketch. I was able to transpose to a part face but that's just an additional capability. When its first inserted to the target plane, the entities are all blue (undefined) because the group is not yet referenced to an origin point or whatever. However it does preserve the sketch entities between each other, kind of like a group. You can lock the sketch into a desired position by dimensioning or alignment. Where I was getting confused is the new sketch does not then turn black indicating fully defined. But I think that is SW way of saying its not, really. Because if the source sketch changes, then the derived sketch updates accordingly. Totally useful. This method saves some copy-paste clicking like I was doing before.

In order to have it fully defined, you just need to lock it down. Lock down rotation and location. Basically it is like locking down a block.