solve for compound miter cut of pipe and placement

Hi again,

I dont see any pipes, just solid bars and bolts..?

Not sure what you want but maybe this helps:

For example when I want to fit pipes together I first assemble them so they interfere and then do the following: 

Model --> Component --> Component Operations --> Cut Out:

First select the part you want to cut, then select the parts that stays in place and Creo automatically creates a Merge/Inheritance of the part that stays inside the part that will have the whole first part as a cut-feature.

Remember this only works when the assembly will stay together..

You might need these settings to get things working:

ALLOW_REF_SCOPE_CHANGE YES
DEFAULT_EXT_REF_SCOPE ALL
DEFAULT_OBJECT_SCOPE_SETTING ALL
DEFAULT_OBJECT_INVALID_REFS COPY
IGNORE_ALL_REF_SCOPE_SETTINGS YES
MODEL_ALLOW_REF_SCOPE_CHANGE YES
SCOPE_INVALID_REFS COPY

I admit - based on your powerpoint slides and from the messages in this thread, I couldn't figure out what you are trying to do.

I guess you are trying to make a miter cut in the pipes so that you can weld them to the square tubing such that when you bolt the flanges together you will have an L shape made out of square tubing and braced with the flanged pipe?

Anyway, here's a link to a youtube video where in its first segment, Leo Greene shows some neat assembly techniques of getting this kind of thing done.

User Defined Features

One of the most powerful aspects of Creo is the ability to make very complex associative sketches.

Considering I do not like external references, I would simulate the interface within the model at the least, and probably do the more comprehensive work in the relavent sketches or other reference sketches.

There are other methods that will work faster and probably even more parametric if you throw out some conventional rules like external references.

One of the easiest ways to get there is to assemble the parts and use the "Merge" function back into the piece part.  Merge is Creo's "booleon operations" function.

Obviously, external sketch references could be done with activating the part within assemblies.

Consider carefully the sustainability of your design.  You can get very messy with your modeling very quickly.

The rule of not allowing external references is the most critical for allowing part files to stand alone without dependencies.

I am still not sure where your problem is.  I assume it is because you don't want to do assembly level cuts.  I'm not a fan of them either, so here is one way of a part model that has external references.

1) Assemble your pipe segments in the assembly - in their final location.

2) Activate the pipe component.  Then switch the selection filter to "Geometry".  Select a face of the rectangular duct to which that pipe will be connected.  Then right click and select "Solid surfaces" icon (it's a cube, I think).  This should collect all the surfaces of the rectangular duct model.

3) Press CTRL+C, then CTRL+V (copy, paste).

4) Open the pipe part now.  There will be a copy feature in the model tree.  Select it, then execute the "Collapse features" command on it (I don't remember where it is - Engineering sub-menu, I think - I suggest you just type "collapse" into the command search box in the upper right).  So, this step will turn the copy feature it into a static independent geometry feature which you can then use within the part to make the cuts you need.  If the duct model is an enclosed volume, then a single "Solidify" command should do the trick.