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joining solids


New member
hello all,

I am an engineering student at Carleton University in Ottawa, Ontario. I am also a mechanical engineering technologist. I used Unigraphics extensively in college, but Carleton uses Pro/E Wildfire 2.0. I am currently designing the superstructure and brake subassemblyof my school's entry for the Great Northern Concrete Toboggan Race (gnctr2005.com). Anyways, I'm running into some modelling problems that most of you would hopefully find trivial. The superstructure is going to be contructed from aluminum piping, both round and rectangular. I have most of it modelled, but it needs some tweaking. I made each section of the piping by sweepingprotrusions alongtrajectories. The pipes are going to be welded together on the sled, and we are going to do some FEM analysis on the frame. I need to know how to join sections of pipe together at the corners and junctions, and trim the excess so the model will appear as it should and so the FEM analysis will be accurate. In Unigraphics, this is easily done using boolean operations such as unite and trim. I know Pro/E doesn't use boolean operations. So if you have two solid protrusionsconverging and you want to join them as one and trim off the excess, what is the equivalent function in Pro/E? Any input would be greatly appreciated, thank you.

(a frustrated student)
Edited by: b_warren


New member
I always like catching you guys at an early point in your Pro/E endeavors. It's true that Pro does not "use" boolean operators but for sake of brevity here you can just consider it to be true. Nevertheless all is not lost. You have some interesting work to do to get where you want to be.

If you have all your parts modeled independently then you will have to do anend-run to get done. Maybe you should e-mail me offline so we don't clog up the works too much.

[email protected]


New member
I see your dilemna. The ol' development of intersections. I have thought of a couple ways to accomplish what you need. If you knew what the angles were of your component connections, you could simply cut your parts at those angles. Straight tubing is much simpler than round tubing. What I did was create 2 rectangular tubes, assembled them and used "Component, Advanced Utils, Cut Out". The results were not complete and I had to add another cut to one of the parts. Maybe someone works with a similar situation and has a tried and true method. I would like to hear what it is.

I also attempted the merge option while in assembly. "Component > Advanced Utils > Merge". This gave me better results, but simply merges one part with another, not what you want.
Edited by: donha


New member
To trim create assembly level cuts refrencing the joining components. This way if you modify the individual tubes (ie. length, angles, etc.), you retiain the proper connections where your tubing meets up.

Does adding welds to the joints accomplish the "merging" of individual components in an assembly?


New member
All the posts describe how you can fix the assy and seems great, but....

I'm not an expert (far from, actually) in analysing welded structures but hope this can guide you to approach it differently.
Since you are gonna use FEA this might drive you into a huge matrix for the solver to work with (perhaps you have acess to Cray's or similar in the university
) and you need to optimize it for that.

For astructure like this is easier not to use the original 3D-model, build a skeleton from the model (points and curves) and use beam elements in your FEA-software and work with symmetry as far as possible.
I would try rigid connections between the beams to model the welds. Some FEA software has support for different weld types as well.

Of course not as fancy as using the 3D-model but a lot faster.



New member
I recommend using surfaces. In WF it's easy to convertsolids to surfaces by usingedit definition on your features that you have already created. Once inside the edit mode you can switch from a solid to surface by selecting the surfaces icon (bottom left hand corner, 2nd iconfromreading left to right).

Modify ("edit definition") both parts so they become surfaces. Then select both of the newly created surface features and usethe surfacing "Merge Tool" , found under the edit menu.

I believe the Merge command will be similar to the Unite command found in UG.

Good luck!


New member
model the individual tubes as solids

put them in an assembly

copy the surface of the part you want to intersect with your tube

use this surface to trim the solid tube.

I used to do it that way to build wheelchair and bicycle frames, the parts will always update when you change angles, positions etc. providing you make the original part much longer than required.