I have a model of a heat exchanger that has very complex bends. We will not be able to bend this out of one length of tube so I need to break up the model into small parts that we can weld together.
When I use Split function I get weird results.
Splitting it here...
...Gives me this part (there are others that are just slivers of the tubing).
Any help would be appreciated.
I am assuming it is a swept profile.
If so with a little work it can be done. On the profile path you can insert split entities points where you need to break it up. You may need to re-assign swept profiles after each split, this is rather hard to explain, but I would try the split entities first and see what that yielded for results.
If you only get your first useable section and have to recreate the sweep for each subsequent section it should not be too time consuming to recreate the part as is only with sections.
Hope it helps.
Why not just do very thin Cut-Extrudes where you want to cut the pipe?
Try this:
Create the entire 3D sketch of the path in an empty assembly.
Insert an empty part in the assembly. Edit the part. Create a 3D sketch, Convert from the original 3D sketch of the assembly to the part sketch, define the length desired (cut what is a "break in the tube". Sweep! For each length that needs to be a separate part, repeat. Create a plane at each segment beginning and end.
Do this for each length (part).
Keeping your external reference selected allows for this to be modified throughout all the changes of the path.
@Paul Risley I do not have the design history tree, this was imported from NX so I only have a blob (dumb) solid. I tried using Featureworks but it keeps hanging.
@Scott Casale I will try Featureworks again and see if I can get it to work.
@Glenn Schroeder I thought about that but wanted to see if I could get the split feature to work. Starting to run out of time so this may be my best option.
@
i assume those 9 planes are intersecting with one another.
may be try one plane at a time.
Here's what the planes look like, just big enough to cover the tube's dia, but in all different angles that, if extended, will overlap and cross other planes.
Planes are infinite in size - they are only displayed smaller so they can be seen on the screen.
if you want to use split, you will need to create surfaces on those planes to limit the extents (size) of the cutting surface.
create a Temporary surface on each plane you created, as shown below.
use surface to split instead of plane.
it worked for me.
when i had plane,it created three bodies,with surface only 2.
see snap shot below.
If you are using the Split function and choosing a plane it will cut through the whole model along that plane for infinity, no matter how big the plane looks.
Unless you choose otherwise. I chose to only split the top chunk
There is my result.
Try is one plane at a time... it might work.
Is the circle shown below interacting with the solid? cutting it?
The original doesn't appear to have this cut or split line.
OR possibly the other planes??
Sarah, good catch! Yes, that was the first attempt I made using a sketch. First I tried the sketch the same size as the tube but it sliced other parts of the tubes so I made it bigger and tried again, then made it bigger than the whole assy and tried again.
Nothing worked as it kept making slices where I don't want them. In your bottom screen shot that was taken before I tried splitting it, so no split/slice lines there.
So I started putting together an assy with the 86 parts the Split function created using the 9 planes and for the first 15 parts it looked good, then I started getting slices that were not right.
Attached is the only way I would do it so you have full control and easy to make. You'll need some adjustment to the sketches (linear) and I only did a partial section
Edit: I did forget to mention one thing - You could add the spiral sketch into an assembly and insert new parts
Edit your sketch and insert split points where you want the parts separate. Then use weldments to create your tube, then you can save out the individual parts.
Thanks for all the help. Since I do not have the history tree on this part I was very limited to what I could do. @Sarah Dwight posts were a great help, thank you.
I didn't end up doing what you suggested because I did not see your reply in time, should have hung around for another 20 minutes or so.
What I did is create the planes where I wanted the splits like I did originally, then extruded small blocks away from the ones I wanted to keep so it would disjoint the body and saved the results as a separate part, then reloaded the original and moved to the next section. It took a little longer than I hoped because the tubes intersected at one point and caused the solid to not disjoint but I was able to get around it quickly. Whole thing took < 20 minutes.
If you are using the Split function and choosing a plane it will cut through the whole model along that plane for infinity, no matter how big the plane looks.
Unless you choose otherwise. I chose to only split the top chunk
There is my result.
Try is one plane at a time... it might work.