CAD Forum

Hello

So I've been using John's SSP approach for a while when drawing assemblies and it works well for me. Lately I've been thinking, what plane do you guys pick when you start a new sketch in a part in one of the sub assemblies, say you want to draw on the front plane and not a plane created specifically in the SSP.

We then have have the choice of the front plane in:
- the main assembly
- the sub assembly where the part reside
- the new part
- or the SSP in all of the above

I've been using the plane of the new part, thinking it may be better if I want to open the part alone, does it really matter?

Terje

I'd sketch in the new part upon a plane in the SSP.
If I really wanted it in the new part, I would create a reference plane in the new part coincident to a plane in the SSP.

Good luck.

The part's plane or the SSP's plane, if the SSP is inserted inside the part. If you do any other, you will create an external reference and create a circular reference.

Thanks

The SSP is inserted in the main assembly and every sub-assembly, not in the parts

Tom G wrote: ↑Mon Jun 20, 2022 10:14 am I'd sketch in the new part upon a plane in the SSP.
If I really wanted it in the new part, I would create a reference plane in the new part coincident to a plane in the SSP.

Good luck.

I know that relations to sketches in the SSP get lost. It's a pain to fix when it happens. I'm guessing external sketch relations to planes are more robust? I've just been pushing coincident planes from the SSP to all my parts recently. It may be more work, but I haven't lost an external reference doing it this way.

temo wrote: ↑Tue Jun 21, 2022 2:44 pm Thanks

The SSP is inserted in the main assembly and every sub-assembly, not in the parts

Enclosure.jpg

The parts that require a reference to the SSP would benefit of having the SSP inserted inside them, rather then having an external reference to an assembly that contains the SSP.

SSP outside of part with links from parts to SSP in assembly = SSP rebuilds, assembly rebuilds, then part rebuilds.
SSP inside parts that require links to SSP = SSP rebuilds, assembly and part rebuild themselves.

Think of it as a tree. Every "level" that is added above the SSP is a tree branch. The more branches you have, the longer it takes to trim your tree. Same thing applies for rebuild. The more branches you have, the longer it takes for the rebuild. If the branches each have multiple branches, then it becomes very exponential rather fast.

mattpeneguy wrote: ↑Wed Jun 22, 2022 8:12 am I know that relations to sketches in the SSP get lost. It's a pain to fix when it happens. I'm guessing external sketch relations to planes are more robust? I've just been pushing coincident planes from the SSP to all my parts recently. It may be more work, but I haven't lost an external reference doing it this way.

It still does. Assemblies higher up still loose the reference. The only way around would be to make a coincident plane to the part plane on the assembly level.

I actually started using more surfacing tools because faces are often more robust than sketches (depends on the design intent though...).

mattpeneguy wrote: ↑Wed Jun 22, 2022 8:12 am I know that relations to sketches in the SSP get lost.

Any idea what triggers it?

jcapriotti wrote: ↑Wed Jun 22, 2022 11:33 am Any idea what triggers it?

Using the mouse with my left hand?...I have no idea...
All I know is that once it loses the reference, and I recreate it, it's likely to lose it again.

mattpeneguy wrote: ↑Wed Jun 22, 2022 11:47 am Using the mouse with my left hand?...I have no idea...
All I know is that once it loses the reference, and I recreate it, it's likely to lose it again.

I was able to duplicate it by editing the inserted model feature, turn off "sketches", then turn them back on. It loses all references to the sketches even when the sketches are turned back on.

jcapriotti wrote: ↑Wed Jun 22, 2022 4:10 pm I was able to duplicate it by editing the inserted model feature, turn off "sketches", then turn them back on. It loses all references to the sketches even when the sketches are turned back on.

Well, that's just asking for trouble. I've never done anything like that.
Usually, it would be upon opening, somewhere up in the feature tree a part sketch would lose reference to a sketch in the SSP. I'd go in and delete the reference, recreate it and it'd be fine for that session...Close out of SW and open it up Monday morning and have to sort it out again.
Other times, it would show an error and I'd have to open that subassembly, and the "conflict" goes away.
Some things work very well in SW and some things don't. Sketch external references aren't reliable, IMO...at least how I was doing them.

I guess I am fortunate. I haven't done much with SSP, but what I've done has been rock solid. There are times I've had the reference part inserted at the part level, and there are other times where the part is driven through a reference in the sub-assembly. It works with multiple configurations (for positioning) and those configurations cascade down as far as they need to. It takes some time to setup initially, but (knock on wood) it works and works well. I do try and keep external references to a minimum. The reference geometry will drive overall dimensions, but everything else happens at the part level.

mattpeneguy wrote: ↑Wed Jun 22, 2022 5:18 pm Well, that's just asking for trouble. I've never done anything like that.
Usually, it would be upon opening, somewhere up in the feature tree a part sketch would lose reference to a sketch in the SSP. I'd go in and delete the reference, recreate it and it'd be fine for that session...Close out of SW and open it up Monday morning and have to sort it out again.
Other times, it would show an error and I'd have to open that subassembly, and the "conflict" goes away.
Some things work very well in SW and some things don't. Sketch external references aren't reliable, IMO...at least how I was doing them.

I wonder if there isn't another factor you aren't aware of. Someone opening the drawing in the new lightweight drafting mode (I can't remember what it is called) or the assembly being opened lightweight. I'm just speculating, but something else must be influencing the behavior.

Thanks, I will look into putting the SSP into the parts.
Will it affect how the subassemblies updates after I do som changes to the SSP out in the process, there is still just one SSP part that needs editing?