CAD Forum

Full disclosure, this may not be possible. But, there are a lot of smart people on this forum so I thought I would throw this out there.

I am modelling pressure vessels. These vessels have various nozzle configurations. They are constructed in solidworks as an assembly with a vessel body, vessel end caps, etc. The nozzles are various threaded couplings. Now, I place them by putting designated cutouts on 8 planes around these cylindrical tanks with extrude cuts in the ASSEMBLY.

That part is all very basic, place a hole on a sketch plane, extrude cut, mate coupling to newly created hole.

However, we often tweak nozzle locations for custom jobs. I can change the sketch plane of the cutout easily enough, but, is there a way to drag the nozzle mating plane along for the ride (used to space the nozzle a set distance away from the cylindrical body). I can certainly manually edit each nozzle mate to the new plane location but I didn't know if any of you super users have a slick way (or can think of a slick way) to make the one edit and propogate that to the mates. I hope I'm being clear.

Here's a shorter version: the sketch plane for a nozzle cutout is also used for a distance mate for the nozzle. Is there a way to tie them together so I only need to edit one plane reference instead of two (or more depending upon whether a group of nozzles should be grouped logically)?

Well, sometimes typing these things out is better than sitting trying to think of it. It may not be the most elegant solution, but it seems to work.

So, its my vessel body that has the 8 defined planes (all the 90's and 45's). BEFORE, I create my cutouts in the assembly, I create a NEW plane called "Liquid Level Switch" or whatever. That is defined coincident to the body plane I want. The NEW plane is used as the sketch plane as well as the mating plane. So, to change both planes I change the definition of the NEW plane to be coincident to whatever the new plane is going to be. I tested it out and it seems to work.

One has to be careful about plane normals and that your cutout sketch doesn't reference anything that could break/not resolve when moved. I haven't incorporated it into all my nozzle locations yet, but I was able to successfully rotate one set around to the various planes. Thanks for observing me thinking/writing out loud...lol!

Not totally sure that I am following here, but if you are making a cutout, then this MIGHT work:

Use the plane to create the cutout at the nozzle level.

Then at the main assembly level, Use the CUTOUT OR THE SKETCH ITSELF to define the position of the nozzle instead of the plane.

That way, when you move the sketch to a new plane at the nozzle level, the mate in the main assembly is using the CUTOUT/SKETCH instead of the plane.

It should come along for the ride.

Thats not a bad idea either and it saves the step of defining new planes just to move them around. I didn't think about using the sketch elements itself as reference for the mate. That might end up being less finnicky with the solver too. I'll test it out.

That works pretty well actually. The only finnicky part is that it doesn't like using the circular arc for the distance to my nozzle face. I had to pick the center point of the arc to apply the distance.

Alternatively, if you have any construction geometry for cutout location that can be selected too. I dimension directly to the circle center for the cutout, but I could put a construction line from the center to the plane and dimension its length. Then it would be available as a mate reference too.

Thanks Dan, works great!

jmongi wrote: ↑Wed Jul 19, 2023 8:30 am That works pretty well actually. The only finnicky part is that it doesn't like using the circular arc for the distance to my nozzle face. I had to pick the center point of the arc to apply the distance.

Alternatively, if you have any construction geometry for cutout location that can be selected too. I dimension directly to the circle center for the cutout, but I could put a construction line from the center to the plane and dimension its length. Then it would be available as a mate reference too.

Thanks Dan, works great!

Glad it worked for you.