Drawing view (intersection of two tubes) 4

[WRH]

I have an assembly model of two tubes. One is a horizontal 2.5" dia tube and the other is a 1.50" dia vertical tube. The assembly looks like a "Tee". My problem is when I created a drawing the "arc line" at the intersection of the smaller tube into the larger tube is not shown. Is this a bug or is there some dtl settings I have to change? I've tried view display and edge display and nothing seems to work. It's also late Friday afternoon and I'm brain dead right now so any help you can provide would be greatly appreciated. Thanks. Running 2001 build 2002180.

WRH

 

[mloew]

WRH,

You have not created any features that will generate the geometry you are looking for. Here are some proposals:

Use an assembly cut feature to remove the intersecting geometry from one part
Use datum curves on the intersection of the surfaces

There are others, but I too do not have much left today...
Best regards,

Matthew Ian Loew

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[im4cad]

I think this happens because what you did is not technologically possible, and probably the software has been designed not to do impossible things. I mean that you cannot create an assembly from two different tubes that intersect each other. You can do it either as an assembly using a whole tube, and the second one would be cut to match the first one’s shape (imagine two welded tubes), or as a “T” part made as a casting for example, when you create the part from two different protrusions perpendicular to each other, or two merged surfaces followed by merge, and Feature --> Create --> Protrusion --> Use Quilt.
In both cases described above, you’ll be able to show the intersection between the two tubes.
I hope this helps.
im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[ohio30]

MLoew and im4cad are totally correct when they state that what you are doing is not correct based on Pro/E functionality.
What I believe you are trying to accomplish is place one tube in space and have the other tube intersect it. Pro/E did exactly what it should have done and did not display the arcs created by the intersecting tubes. When you intersect solids in an assembly you will see strange things happen at the intersections because two solids cannot occupy the same volume.
One way to get your arcs is as follows:

1) Keep the vertical tube model (.prt)
2) Open the horizontal tube model and "Save As" to a new file name that would suggest a weldment (i.e. tube_weldment.prt)
3) Create an empty assembly model (file name is not important, since the assembly will never have to be opened/used again.)
4) Assemble the vertical tube part in the assembly (the part should place itself, since you do not have any assembly planes or csys).
5) Assemble the new horizontal tube model (tube_weldment.prt) using valid assembly constraints. Be sure that the constraints are "fully constrained&quot
6) Select Component--Adv Utils--Merge
7) (prompt: Select parts to perform MERGE process to.) Select the last model in the model tree - tube_weldment.prt
8) Select Done Sel from the pick menu
9) (prompt: Select reference parts for MERGE process.) Select the first model in the model tree - vertical tube
10) Select Done Sel from the pick menu
11) Select Reference--No Datums--Done
12) If prompted to exlude/remove part from assembly - accept the default response (yes).

You now can draw the intersecting tubes using the tube_weldment.prt model. Note: Any changes made to either the tube_weldment.prt model or the vertical tube model will be reflected in the tube_weldment.prt model.
This will do it!
Althought, you have not described any other reason why you could not use this method I would perform a test merge before committing to it.
The merge utility is great, but if you need BOMs or dimensions on the drawing from the vertical tube model (show/erase) you will have to work hard to get them.

Tip: To modify the vertical tube features from the tube_weldment.prt use Query Select. The Query bin will display the merge feature first and then the following features will belong to the vertical tube model. The same would apply if you need to show/erase dimensions for the tube_weldment.prt on your drawing. Try using Sel by Menu to get to those hard to reach dimensions.
Another problem with the merge feature is if you have any cosmetic features or datums curves on the vertical tube model (refernce model) they will act as a single feature in the tube_weldment.prt This means that you cannot show/erase the cosmetic feature on the drawing as if it were a single feature. If you want to exclude any item belonging to the vertical tube from the tube_weldment.prt I would suggest that you create a layer and place the merge feature on this layer. Blank the layer and Save status. This is great if you have datum curves that are not relevant to the tube_weldment.prt model.

Hope this helps? Too much information is better than not enough when speaking on the subject of Pro/E.