"bending round or tapered stock.

[brudje]

I have been trying to put a jog into a tapered round profile. The flex feature give no predictablity at all. each time I change one bend the other is out of wack. I tried using a sheetmetal feature, but this doesn't like the round base feature either. For such a simple thing I am have spent way to much time....Any thoughts would be appreciated.

 

[ctopher]

Can you show a pic of it?

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[brudje]

I hope this worked...

 

[smcadman]

It is because you are using the wrong tool. What you need to do is sketch the path of the "tubing", and SWEEP a circle along the path. The cone shape can either be revolved or extruded with a draft.

Flores

 

[Theophilus]

smcadman is correct. Create a path along which to sweep and use a radius to connect the straight lines in the path.

Create a guide curve (to represent the top tangent line of your swept feature--or bottom, or side or whatever you want) that follows your path. The radii on the guide curve must be concentric with the path radii or the feature will crash into itself as it moves along the path (logic problem). So your path radii must be large enough to accommodate this.

Create a circle normal to the path, pierce the center to the path and the edge to the guide curve (may need to add a point coincident to the circle edge to pierce to guide curve).

Your feature will be as you need.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[ctopher]

I agree with smcadman and Theophilus.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[brudje]

Thanks for the response guys. True, that that will give me the end geometry I am looking for!!!
I was hoping to be able to use a feature that I could easily suppress so I can put the initial lathe/tapering operation on a print and use the bent as the final form. That is why I was pursuing the flex/"bend" so I could maintain a flat state prior to the bend....
I will work it out

Thanks again....

 

[CADGemini]

brudje,

All you need to do is create a configuration to have one represent the bent and one to represent the flat. you will probably end up with twice as many features in your tree but this can be done.

Best Regards,
Jon

Challenges are what makes life interesting; overcoming them is what makes life meaningful.

Solidworks 2005 SP3.1