In a single part file I want to create a fabricated hollow section framework built up of many extruded features. The problem is that each extrude is automatically merged together where they touch showing no join line. I would like all the join lines to show up in the part model and drawing file so that the welding fabricator can see where and how I would like the frames to be welded. For example, 90 degree connections or mitred corners. I basically don't want each extrude to join up automatically. I know leaving a very tiny gap at each connection will stop this happening but this can't be good practice and is time consuming process.
I don't want to have to create an assembly of all the various tube lengths so that they show up seperately.
What you are looking for is multi-body parts. That is NOT something that Creo does.
In Creo your process would be to build all the components as parts and use an assembly to put them all together.
NX (Parasolid) allows multi-part bodies in a single file. Creo (Granite One) does not.
We had the same issue where I used to work with welded structures when we switched from Unigraphics to Pro/Engineer. We would model the welded structure in a single UG part file made up of multiple extrudes. When we switched to Pro/E, we had to do the individual tube files and an assembly for the welded structure. We just assigned (-xx) part number suffixes to the tubes and did not use them in any other assemblies. If we needed the same size tube for another assembly, it was either remodeled or we did a save-as. Since we were building to manufacturing orders, we did not stock (or sell replacements) the tubes.
From what I have found on the internet so far, it looks like the only option so far.
I've used multi-body "parts" for rough concepting work. I'll make each extrude/revolve/sweep/etc. a surface feature with capped ends. The features won't merge into each other without you telling them to (via quilt merge).
I use this method just to quickly iterate a design to see what's possible. After I settle on a direction I may use the surface model as a skeleton to create individual parts.
A couple downsides to this method is that you won't be able measure any mass properties or generate BOM's from the surface model. Works for me since I don't need those for concepting.
You can model using gaps, which will typically be present in pre-weld fitups. Alternatively create datum curves to represent the separations. Both are more tedious than a feature that Creo doesn't have, but they are available.
Keep in mind that in an actual weldment there will be no gap and it will tend to look the way that Creo defaults to.
Have you looked at AFX (advanced framework extension)? All seats include a "lite" version which includes full functionality but assemblies are limited to 20 items. With some creativity in splitting your assy up into sub-assys, you can get around that.
It's made for welded tube structures and has all the features for placing them and doing all the miter cuts. It's a bit quirky, but if you look up the how to videos on the Learning Exchange and you should be able to pick it up pretty quickly.
I tried the surfaces and capped ends and you are right, it will work for concept work. I will be able to use this for some of my projects. It's a shame that it does not let you add holes into the frames for fixing outside guarding to and other items.
Great suggestion, thanks.
I have used gaps before and also thought about curves. Like you say, they take a little longer.
I only tended to use a very small gap that is hardly visible. I am trying to go away from this method.