Tube and Pipe "sweep operation failed"

[Tim.Malkowski]

Hi,

I am new to tube and pipe and I am just getting to grips with it.  So far I have been getting on not so bad.  I seem to be hitting a brick wall with this aspect. This is producing hoses.

What I have done is produce a new flexible hose style.  This is a copy of a existing one and I have suppressed one of the end fittings as i do not need it. For info it is a 1/2" hose min bend radius 180mm,  hose round up 10mm.  So I create a new route and start to  place my route. Just using the start and end point.  If I finish the route there and populate route it works fine, but the hose is not in the position i need.  So to get the hose the way i want it I add a insert Node and use the redefine option to connect it to a work point i set up before.  The hose path looks good, but when I finish the route and try and populate it I get an error message saying the sweep operation failed.

I have attached a couple of picks to show the hose and the error message.

Is there a step i am missing?  Any help on where i am going wrong would be great.

 Also if anyone knows of any good self teaching material for tube and pipe that would be useful.

Hose made from 2 point that will populate.

Hose with 3 point that will not populate

[smokes2998]

Check if you have a sharp corner in the route the best way to do this is hide everything but the route and look through it you should see a sharps straight intersecting line it is really small

It is also dependent on the minimum hose bend radius as well.

There should be  a 300 page  pdf document in the autodesk inventor install directory on routed systems it covers most of T&P pretty well.

[Tim.Malkowski]

Thanks for the suggestion.  I starting to find this very frustrating.  I have done what you suggested and i have had a close look at the hose path, and it does seem that there is something double backing on it self very tightly where i have put a node.  Would this have something to do with the 0.1 dim that comes up at the nodes.  see pics

[Tim.Malkowski]

Thanks for the suggestion.  I starting to find this very frustrating.  I have done what you suggested and i have had a close look at the hose path, and it does seem that there is something double backing on it self very tightly where i have put a node.  Would this have something to do with the 0.1 dim that comes up at the nodes.  see pics

[smokes2998]

that will do it you need to delete a the nodes that constrain the spline. It is an utter pain but you have to try and use the minimum amount of nodes to constrain the hose.

[Tim.Malkowski]

Thats not really that much help.  I think i must have something wrong in the setting or the way i am working.  As i am trying this in different places and i can never get it to work with more than 2 nodes.  I have watch a number of vids on making hoses and I cannot get it to behave the way it does on the vids.

[Anonymous · Accepted solution]

HI Tim, just for the record,

Thanks for taking time out to watch the trick.

The basic procedure I did was…………..

1. In Model Browser, navigate to Tube & Pipe Runs > Run11 > Flexible Hose18
2. Open “Flexible Hose:1”
3. Turn On Visibility of Work Plane 1
4. Create Offset Work Planes about 1” apart from Work Plane 1
5. Create Sketch on each new work plane & Project the Geometry that is the centre Point at the end of the Hose Opening
6. Go Back to the Assembly & Turn On the Visibility of the two new sketches you just created
7. Edit the Hose 18 Route
8. Create Grounded Points at all three visible points
9. Create three nodes along the existing Spline
10. Create “Co-Incident” Constraints between the three Grounded Points & the three corresponding nodes on the Spline
11. Finish the Route & Update the Assembly
12. Repeat the same on any troublesome hoses

Hope that makes sense.

Cheers!

Steve.

[blair]

The doubling back will most likely cause a self intersecting sweep which will cause the route to fail. Also minimum segment lengths where a segment is less than the Style setting.

Somethings with a specific route, you just end up deleting the run and creating a new run.

I will use the "Dim" function in the T & P to dimension the work point to the model geometry. I find this is easier to work with than creating offset work planes.

When you are editing the run, in the tool bar you will see a small "dim" icon. Use this to set the dimensions from the work point to model geometry.

[blair]

I didn't add any dimensions just to knock it out quickly.

Single part, uniform wall thickness through.

http://autode.sk/2b8XKFz