OK, I'd really like to show the holes in this pipe where the couplings are welded in. Any ideas? One would suspect there's an easy way to make this happen, but I've had no luck...
Sketch either in the corrosponding plane of the pipe part or in the assembly and extrude the cut through the pipe. In the assembly you can filter bodies to cut so you don't cut through your coupling.
Scott/Robert - thanks for the responses. I'd prefer to have the cut show up in the part, but SW protects the pipe parts - it won't let me add a cut from within the pipe part. Here's the message I get when I try to add a sketch to the pipe part. I get the same message if I directly open the pipe part itself and attempt to add a sketch.
I did have success with creating a cut from within the assembly, but if I want to show the pipe part alone on a drawing (so the holes can be dimensioned) they don't show up. I was writing to see if anyone had found a way to circumvent SW's pipe part restrictions.
I wish solidworks would ease up on the pipe part restrictions (another topic, but it would also be nice to associate mates in higher level assemblies to pipe parts).
Yeah, I get it now. You could make the hole features part of a configuration of the part that you can toggle off and on based on use so it doesn't conflict with other places the pipe's used.
Also did you know you can use that assembly in a 'part' drawing and suppress the flange in the view? I use that a lot when I have features specific to an assembly and want it shown on a part drawing. Kinda cheating, but it works and more importantly, boss-pleasing quick.
Couple of ways you can do this Tommy;
1. Add a ref. plane at the end of that sketch line you have sticking out of the pipe, cut-extrude a circle sketch from there onto the tube. If the sketch belongs to the flange part, you may still do this in-context of the assembly.
2. Use whatever plane running along the axis of the pipe, start an extrude-cut circle sketch and blow through the pipe wall. If your plane is not clocked right in relation to the couplings, add a ref. plane and create your sketch there.
Welkom in the world of routing piping and SW.
(I really hope you are going to enjoy it alot more then me....if it works, its brilliant....if not......your f*cked for real....)
I dont know how large your assembly is but you could work around the problem by using the same assm. cut solution you already modeled an make a display state that only showing the pipe (make the display state -> select all part -> hide -> unhide/show the pipe.
The sh*ty thing is that this wil make you drawing heavy(er). (But this can be solved with an invesment in hardware)
Display states have alot of .... how do I say this nice.....well lets call them issues ....
So please check your 3d file before going wild with this.
things to test:
Will all display states still show the correct part/thing when you at/ edit / remove / replace others
If thing appear like: "Where the h*ll did everything go?!?"
Lightweight ..... should work, but sometime features created in the assembly will not update to the drawing. (also check you printed drawing it they do apear on the screen)
If you dont have a lot pipes that need holes I would chose a different approach....
1.)And planes parallel to the face of the flanges on the Cpoint \
(skip this step if the Cpoint is "in line" with the end face of the flange (if you have no welding gaps)
For the info -> I did this in my "library part"
First route everything (dont place any parts/fittings on the pipes)
At lines parrallel to the route (in the routesketch) where you need/want the holes
2.When you route is done; make the lines (in the 3d skech of the route) "for construction only"
Update the route -> the pipes on the "for construction only" line should be removed....if remove them by hand (just remove the pipe in the feature tree)
Drag in the pipe that you used for the route. Open it -> safe as (I save them to the project folder were I keep the project related files)
Mate it in place -> change the extrude length -> and now you an ordinary part in with you can cut/slice/spit ect all you want.
I hope one of the 2 will get you were you want.
Ha! I'm in agreement with "if it works, brilliant; if not, you're forked..."
I don't know if the SW folks will ever see this thread, but it would be nice to see better functionality with regard to inserting couplings into pipe. Weld-o-lets are cool, but we don't use them. Also, I find tyring to use weld-o-lets in SW difficult. And yes, I've tried faking couplings into thinking that they are weld-o-lets, but I would have to create a configuration for each coupling for each diameter of pipe that it could possibly be used with. That's not going to happen anytime soon.
DEAR SOLIDWORKS: I envision a "coupling function" similar to the penatrate command. Draw a line perpendicular to the pipe run and let that be your coupling location. Choose a coupling from a qualified list of couplings, and SW will insert it and automatically add the proper hole in the pipe. That would be cool.
"...if it works, its brilliant....if not......your f*cked for real..."
LoL, ain't that the truth !
Couplings, even the ones that you get by just installing the premium version, are not piping elements. This isn't me saying so but SW employees themselves who work in the Routing department.
The mind boggles, I know.
The only way I have found to work is by going on Pipe assembly level and by using normal mating techniques adding them there. The reason being that if you are on Pipe assembly level then it doesn't recognize the assembly any longer as being Routing and there for you have lots more freedom to do what needs to be done. Even if it's something as unheard of as putting socks and nipples perpendicular on a pipe for instrumentation purposes. Gosh, why would anyone ever want to do that, eh? Also, yes it is necessary to create configs for each kind of weldolet, in each size for each size of pipe you want it to be mounted on but ..... thankfully design tables work a treat for that, i.e. I only have one of each (nipple, sock, etc) but each one do have a nicely sized design table incorparted.
Concerning holes in pipe, the only way that will work directly in routing, without having to result in real hairy stuff, would be by adding a pipe in the location of the nipple - sock - weldolet - etc and then use that pipe do a penetrate, afterwhich you hide the pipe as well as making sure that it doesn't show up in the BOM. I must admit that I don't bother with it because even if you do get the hole that way there isn't much you can do with it, dimensioning wise.
Have a nice one and good luck with it.
I like the picture you shared - very illistrative of the fact that welding couplings perpendicular to pipe runs is a common occourance.
It's always interesting to hear how other folks "work around" issues like this. Even if there's not explicit functionality in the software to solve a common design problem (like welding couplings into the side of a pipe) it seems there's always at least one work-around, usually several.
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