Trying to create an assembly feature - sweep to create a wire

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

Hello,

 

I'm trying to create an assembly feature that is a sweep of a power cord cross section along a 3D sketch.  I have tagged the assembly as a weldment to enable the sweep command in assembly features.  I created a 3D sketch with radii that should be large enough to allow the cross section to follow it.  When I try to create the feature, it fails.  Is that becuase the command is only set up to sweep weld fillet cross sections?  

 

In the attached image, you can see the 3D sketch and profile I'm working with.  There is a power cord sweep that is in the model, but I had to do that one by moving the plugs to a subassembly and then create the cord as another part with insert part copy faces to drive the feature.  

 

The 3D sketch is created in the assembly.  The power cord cross section is also a sketch in the assembly.

 

Assembly features - wires.JPG

 

Any ideas on what I'm missing or doing incorrectly to create an assembly feature sweep?

 

Thanks!

 

Kyle

Kyle Joiner
IPA LLC
ST9 MP1
17 REPLIES

Re: Trying to create an assembly feature - sweep to create a wire

odd,  i just tested too in ST9...  looks like even though you go to toold and mark as weldment that the sweep is not there.

 

BUT.

 

just to the right of sweep in assy features tab is a weldment tab.  if i clicked that and remarked the check box as weldment then it took and the command became active...??

 

HTH

===================================================
Matt Johnson
Solid Edge Certified Professional (ST7 & ST8)
Solid Edge ST9 (SEEC) - Production
NX10 (Tc Integration) Pre-Production Testing
Teamcenter 10.1.6

Re: Trying to create an assembly feature - sweep to create a wire

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

Hi Matt,

 

The "mark as weldment" check box appears to be the same when going through the tools tab or the welmdent tab.  It should be the same button.  The sweep tool goes through all of the steps and allows me to pick the 3D path and then the cross section, but it never creates the feature. It shows as a failed feature in the assembly features section of the pathfinder, however.

 

Kyle

Kyle Joiner
IPA LLC
ST9 MP1

Re: Trying to create an assembly feature - sweep to create a wire

gotcha... sorry, assumed the feature was not exposing...
===================================================
Matt Johnson
Solid Edge Certified Professional (ST7 & ST8)
Solid Edge ST9 (SEEC) - Production
NX10 (Tc Integration) Pre-Production Testing
Teamcenter 10.1.6

Re: Trying to create an assembly feature - sweep to create a wire

Phenom
Phenom

Hi @kjoiner

 

 

this is an issue where I would use the structure frame as tool to create the swept protrusion.

 

define the cross section of Your cable as a part with one protrusiion an use it for Your cable.

 

Structure frame is a function I have used many times for cables, pipes, frames of course and belt drives for example.

 

.

 

 



regards
Wolfgang

Re: Trying to create an assembly feature - sweep to create a wire

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

Hello,

 

I'm really interested in just creating assembly features so I don't have to create extra parts and subassemblies.  This is mostly for a graphic representation of the cord.

 

Kyle

Kyle Joiner
IPA LLC
ST9 MP1

Re: Trying to create an assembly feature - sweep to create a wire

Phenom
Phenom

Hi @kjoiner

 

 

a structure frame only exists in the assembly, so more or less it is an "Assembly Feature"

 

 



regards
Wolfgang

Re: Trying to create an assembly feature - sweep to create a wire

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

Here is a Jing video illustrating my attempt at creating a swept assembly feature:

 

https://www.screencast.com/t/yho0QCz1vJSn

 

 

Kyle

Kyle Joiner
IPA LLC
ST9 MP1

Re: Trying to create an assembly feature - sweep to create a wire

Phenom
Phenom

Hi @kjoiner

 

 

I have understand what Your intenation was, and after testing it here with ST9 - MP6 I have seen that a swept protrusion as assembly feature even isn't available as feature as long as there is no part in the assembly.

So I suppose that a weld feature has to be somehow in contact with another part body and will only be created if this is true.

 

Again, the only way I see at the moment is the use of structure frame.

 

For me it yet is the easier way to get the cable in.

You only have to define the sharp edge path of the cable cord, click it, choose the cross section (you only need one part with one sketch in it) an apply that to the cable cord.

Done!

Another advantage IMHO is, that those cross sections are associative connected to the frame elements.

Changing them will change all Your cables based on the same cross section.

 

And as mentioned, the cable cord structure frame only exists within Your ASM.

Similar to the ASM feature

 

 



regards
Wolfgang

Re: Trying to create an assembly feature - sweep to create a wire

Phenom
Phenom

Hi @kjoiner

 

just conitnued with my test here and immedieately after placing the sketch onto a part face the swept protrusion will be created.

 

Okay, and here is what I think:

 

I have one rule for such situations:

"If one method doesn't work or will not succed

I always hope to have a second way which leads me to the goal!"

 

And as long as the sweeping will not work as I need it,

I happily would use the frame command.

At least it let me finish the task.

 

 



regards
Wolfgang