Swept Cut Normal To Sheet Metal

Hi there!

I'm trying to cut a open through a sheet metal part based on a swept/spiralling tube.  It's a bit hard to explain what I would like to accomplish, but here goes:  I would like to end up with a cut that is normal to where the tube meets the sheet metal on the underside, as well as where the tube exits on the top surface of the sheet metal.  I tried cut with surface but the result is not 'normal to'.  I also attempted to use the 'Intersection Curve' to create a sketch I can cut 'normal to' with but this only gives me half of the result I'm looking for.  In the example attached, the cut is normal to where the tube exits the top surface.  Any suggestions would be much appreciate!

Thanks,

Paul

SolidworksSheet Metal
Answers 9
SF
SF 2012-06-22 Best Answer

Sorry, this file is a SW2011 version file and any reply examples would be much appreciate in that version.  Thanks!

SF
SF 2012-06-22

Hi Paul,

why u are not using sweep cut...

SF
SF 2012-06-22

something like this?

sorry was 2012 file

add a sketch to the otherside of the sheet before the last cut extrude,  convert with intersection curve the shape, change the sketch of the cut, and convert the entity of the just added sketch.

SF
SF 2012-06-22

Hi Jan ,

Still cut out is coming normal only it is not cutting in the form of tube..

DL
DL 2012-06-22

Jan - Paul

Jan's answer sounds right. Here's a SW2011 version, I think, attached.

Here's an image.

Dwight

comment imagecomment image
SF
SF 2012-06-22

Jan/Dwight:

This appears to be a method that would solve my problem.  However, I'm having problems creating the tangent relation between the two curves - my sketch becomes unsolvable and I cannot reproduce your method.

Here is my order of operations and the unsolvable sketch result:

  • In a first sketch, I created the intersection curve between the tube and the sheet metal bottom surface
  • In a second sketch, I created an intersection curve on the top surface
  • Still in the same sketch, I convert entities from the sketch on the bottom surface
  • I draw a line between both curves and assign a tangent relation between each end of the line and adjacent curve, and repeat for the other side.
  • Using trim entities, I can trim the curves and lines down to the representive slot but my sketch becomes unsolvable

I think this is a logical approach, am I missing something in the sequence?  Is it a limitation in SW11 perhaps?

Please advise.

Thanks,

Paul

SF
SF 2012-06-22

Not sure why the outside tangency matters since it's outside the material you are trimming, but you have your reasons I'm sure.

I had the same issue you did with making ALL the end points tangent. I believe it's because of the intersect spline on the bottom defines the endpoint. I was able to fully define the sketch, but only making the inside line tangent and the trimmed end of the outside line. Hope that makes sense...see sketch.

DL
DL 2012-06-22

Paul

I was able to make all 4 ends tangent. Be sure to 1) convert the curve from the first sletch to the second sketch and 2) apply tangencies to the converted curve and not the curve from the first sketch.

Dwight

EB
EB 2012-06-22

Paul,

If I understand what you are trying to do, it looks like you have a handle on it.  I've run into similar situations.

One thing that comes to mind is how are you going to make the part in "real life"?  I have usually had to find the closest punch that was available and make my hole that size. If you are going to have the part lasered (or plasma or waterjet) you still want to find the closest true arc, so using a spline formed by the intersection is not much help in the long run.  Just make an obround and adjust the size and location to fit on both sides.