Trouble with Cut Extrude

[robperly]

Hello,

I have been having this issue quite a bit, I'm not sure if my technique is wrong or I am just going about it the wrong way.

In the picture below I am trying to do a cut extrude to remove the small nub, however I can only 'blind cut'. If I try 'up to surface' or 'offset from surface' I recieve the error 'the intended cut does not intersect the model', when the cut does intersect the nub(model), which is part of the overall solid body?

Any thoughts or tips appreciated.

 

[Theophilus]

Is this an imported model/surface you're working on? If not, roll back to before the "nub" feature was created and knit together all the surfaces in that area. Roll back to where you want to add your cut and use a surface cut with the knit surface instead. If the surface cut doesn't work, use an extruded cut up to your knitted surface.

The cut doesn't work the way you're intending because you're specifying a surface totally outside the bounds of your extruded profile. Also, the surface doesn't envelop your extruded profile even if it did overlap. So SW doesn't know what to do, since your cut is being specified somewhere your sketched profile does not truly concern.

Try the workaround I mentioned and I think you'll be fine.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[robperly]

Jeff,

thank you for the reply, unfortunately the model is imported geometry (parasolid). I now understand why the cut is not working. Is there another I can try to cut the small nub feature to blend with the existing surface or can I only do a blind cut and then add a radius to match whats there?

Thanks,

Rob

 

[J-C]

Is there more than one body in the file? Instead of letting it Auto select it, expand Feature Scope at the bottom of the extrude dialogue and uncheck Auto and manually select the body you want it to affect.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP0.0 on WinXP SP2

 

[dgowans]

Another option would be to try the Delete Face (Insert, Face, Delete) command. Pick all the faces of the "nub" and make sure the "Delete and Patch" option (default) is specified. This will yield the cleanest geometry if SWX will extend the surrounding faces. The other options of the Delete Face may work for you, depending on what you're trying to accomplish.

Dave Gowans

 

[Theophilus]

Dave, that's a good point--often works best when you've got imported geometry. In this case, I would delete the nub faces wihtout filling or patching, then fill the hole as a separate operation to control surface tangencies.

It looks like the nub remains primarily on the fillet, but extends onto the non-fillet surfaces. This may require a fill in two steps with surface trims/extends first (complicated to explain here).

Rob, if you have difficulties after trying it out, you can send me the file by email and I can fix it and send it back. My email address is on the contact page of the site below.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.