Best way / tipps to design pipes in context 1

[Donnis]

Hello everybody,

can somebody give me some advices on how to make pipes in an assembly (industrial installation)? I think I have to use "design in context" because the pipes are linking different equipments and the paths are not very simple. I'm working with SW Office 2006 - so the routing function is not yet available. I'va started to make pipes as sweeps with "thin" option activated, based on 2d sketcher or, where no other possibility, 3d sketcher (I try to avoid working with 3d sketches because for me there are not so easy to control as 2d sketches). Maybe somebody has some "best practice" advices for me?

Thank you very much in advance!

Donnis

 

[Eltron]

Routing would be the way to go if you can get your hands on it. Otherwise you have the right idea. Create sketches and sweep profiles along those paths. I tend to avoid 3D sketches as well in general design, but this is one application that 3D sketching will be a benefit. So, don't fear the 3D sketch...embrace it.

Dan

http://www.eltronresearch.com

 

[ctopher]

I agree with Dan. Without using Routing, the 3D Sketch is the way to go. It may be cumbersome at first, but you get used to it.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated 10-07-07)

 

[JMirisola]

It's really helpful to split your screen when using 3D sketching. Not only can you better see which direction your sketching, but by moving your cursor to a different view, it'll change the direction as well, versus just hitting the tab button.

Jeff Mirisola, CSWP, Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo, 4GB RAM, Nvidia 3500M

 

[ShaggyPE]

Tab is your friend with 3d sketches. It changes the x-y, x-z, y-z plane you are sketching on.

If the pipes are primarily pictorial and you don't have to make an assembly of fittings and such, my recommendation is to model the pipe network as a single (probably multi-body) part. In the context of your assembly, just use sketch relations to locate sketch points to key locations. Then back in the part, do your 3d sketch, connecting the dots and continue with your thin feature sweep.

-Dustin
Professional Engineer
Certified SolidWorks Professional

 

[Donnis]

Thanks everybody for answers. I'm starting to get used with 3d sketching and the results are very good!
A further question would be what is the use of a sketch made directly in assembly (without creating a new part or editing an existing one)? I'm confused because normally it should only be possible to create sketches in parts, but not also in assemblies!?!

Donnis

 

[ctopher]

It's an in-context part. It's easier to build your pipe within the assy...you can see the other parts while routing your pipe. It still becomes a separate part, but is tied to the assy. It can be broken if needed when completed.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 06/08
ctopher's home (updated 10-07-07)

 

[ShaggyPE]

I think Donnis is referring to the ability to simply open a new sketch in the context of an assembly. These sketches are typically created to generate assembly level features. Assembly level features can only remove material, not add... so only cuts are allowed.

An example of an assembly level feature is if two parts are bolted together and then a match drilled dowel pin hole is added. The two parts would not have the dowel hole... the assembly would.

-Dustin
Professional Engineer
Certified SolidWorks Professional

 

[Donnis]

Thank you all, specially ShaggyPE - it is exactly what I mean. Now it is clear for me why I am able to create sketches in assy context. ShaggyPE, I gave you a star for that! Thanks again!

Donnis

 

[zirtapoz]

Insert a new part to your assembly. Edit part from your assembly. Use 3D sketching and weldment. While you use weldment you will have separate bodies automatically. With weldment you can do everything with a part file. You can make pipes, valves, flanges, every thing yo need. You can combine bodies, copy,move them to other sides. You can manage your feature, face, body colors. Then you can get a list of your all bodies with quantities. With 3d sketch you can manage your design more easily.You can organize relations easily.

 

[madvlad]

From what I learned doing something similar (a redesign of an aircraft system, involving rerouting/design of some 450 hydraulic tubes):

SW Routing is clunky, slow and overcomplicates things sometimes. It's not meant for aircraft hydraulics, which is what I was doing. Maybe for a couple steam pipes with 90 degree fittings, flanged fittings etc, it'd be better.

Skeleton parts (containing lots of 3d sketches) driving an assembly of tubes worked well for me. This allows you to group a bunch of tubes parallel to one another, and easily move that group around during redesign.

3D sketches are not very robust. If theyre too complicated they fail to rebuild. If you put radii on everything, it has a hard time rebuilding if u move stuff around, especially if youre not along global XYZ. This is one area where CATIA blows solidworks out of the water.

For in-context, dont use convert edges to get lines. Draw the lines from point to point (ie coincident relations), it rebuilds way better, especially when you apply radii. Convert edges is actually some sort of clunky collinear relation with ambiguously defined endpoints.

save bodies can be used to split a run into individual tube segments. Name the solid bodies before you save them, with part numbers, so that you can call them up on the drawing with balloons without having to look anything up...saved so much effort.

Anyway thats what I did, hope it helps
Chris