Designing with tubes

You could model the part as solid rods instead of hollow tubes. Then use the Shell command and select all the end-caps as surfaces to remove.

ArtW

Extrude a "rod" with "Up to Surface" , and then do the ID cut with "Up to Next".

Bo

If you were on 2007 perhaps you could use multi bodies part and subtract small pipe bodies from the big one

in a word, weldment.

as far as the cuts in the small tubes, you can simply make a sketch on the end of the big tube and use it to cut off (notch) the ends of the small tubes. you can do the same thing by making a surface on the big tube and using it to do a similar cut.

As far making the holes in the big tube, more info is needed. Will the holes be made with a drill type of process (hole ID concentric to small tube) or will the cuts be done with a laser or saw? In the latter case, you may need to deal with wall thickness.

Also, depends what you mean by "automatic".

Bill

I have done in past years a vacuum chamber with dished heads that had multiple ports that were focused on a point or points inside of the chamber. Of course these were all water-cooled so the pass-through hole had to pass thru multiple layers. We used a long tube, one end mated to the focus point and the other end would float so we could add all of the required tube pass thru's and make room for all of them on the dished head of the chamber. Once we got them properly placed, we would cope them to the interior leaving enough extension for a fillet weld. Then we had to cut holes manually. In SWx 2005 you are limited to this kind of manual processes. In current versions, you can make library parts that have a feature that can do this cut at the same time. Weldments may also be better suited for this purpose. You may still have to cope pipe pass-thru's so it is symmetrical to the interior of the chamber, or not depending on your application. iQ

I was able to do this in 2004.

In the assembly of your tubes with the main tube initially placed:

1. Create a 3D sketch as a skeleton to orient the intersecting tubes.
2. Mate the intersecting tubes concentric to the 3D sketch.
3. Create an offset surface from the inner or outer wall of the main tube to delineate the surface to which you want to trim the intersecting tubes and hide it.
4. Edit in place the main tube.
5. Using the TOOLS/SKETCH TOOLS/INTERSECTION CURVE command pick the outer surface of the main tube and the outer surface of an intersecting tube while holding down CTRL. This will create a 3D sketch curve at the intersection.
6. Ditto using the inner surface of the main tube and the outer surface of the same interecting tube.
7. Pick the two 3D sketches and use the INSERT/LOFTED CUT command to punch a hole in the main tube.
8. Repeat 5-7 for each intersecting tube.
9. Edit in place an intersecting tube.
10. Offset the surface created in 3 by zero.
11. Pick the offset surface and INSERT/CUT/SURFACE trimming the tube.
12. Repeat 9-11 for each intersecting tube.
13. Lock external references for each tube cut in the previous steps.

TOP

Yeah, this is a vacuum chamber, too (though not a water-cooled one).

But I've now got the knack:

1. In assembly, make a (possibly 3D) sketch with a line that goes from focus point to flange plane

1. Bring in flange part and mate with sketch line/endpoint

2. Edit part "Main tube", insert sketch on flange weldment plane

1. Draw 2 circles coradial with the inner and outer perimeter of the annular tube mating surface of the flange part

2. Extrude sketch "up to next" (this makes a stub attached to the main tube)

1. In the chamber part, insert sketch on end face of just-created stub, draw circle coradial with inner diameter

2. Make an extruded cut with this sketch, "Up to next".

Sounds complicated but just takes about one minute per flange. What's important is that the position and orientation of the flange are entirely defined in step 1.

Thanks evberybody for your replies!

--Daniel