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Solidworks: extruded cut but not normal to the sketch plane?

Strostkovy

Titanium
Joined
Oct 29, 2017
I have a shape in a wall of a die cast part. The wall is at 45 degrees from the die closing direction. Is it possible to take a sketch of the shape I want, on the face I want it, and then extrude it in the direction of the die closing, with draft angle? I would be extruding the cut 45 degrees off axis of the plane the sketch is on.

I can't seem to find a way to specify an extrusion axis for bosses or cuts.
 
If I'm understanding correctly, you should be able to create a plane on the 45 degree axis. If you use that plane to create your sketch you should be able to drive the cut normal to that with all the normal options/features
 
I believe what you may be looking for is a loft cut… it’s been a while since I’ve been on solid works, but you may have to draw some helper geometry… I.e. if you want to loft cut to a feature at 45degrees, you may need a center line to follow, as well as a sketch of what the feature looks like on the 45 deg wall.

I can get on solid works at home if you have more details of the exact feature
 
If I'm understanding correctly, you should be able to create a plane on the 45 degree axis. If you use that plane to create your sketch you should be able to drive the cut normal to that with all the normal options/features
The trouble is that I can't make the geometry on that plane without extreme difficulty and have the cut at the face be correct.
 
It seems like a lofted cut can do what I'm wanting in what feels like a functional but overly complicated way.

It can also do a whole lot of things I don't want..
 
Perhaps it would be better to post an example of what you want... Just guessing here....
Can't you make a plane normal to the die closing direction, project the sketch from your 45deg wall, then extrude it normally?

Here is a circle drawn on the 45deg wall, projected onto a plane normal to vertical, then extruded vertical (so that the profile is actually an oval). You can then use the "draft" function.

But maybe this isn't what you're asking for....

Sketch on wall:
1713474223036.png

Projected vertically:
1713474393294.png

With draft:
1713474436660.png

From above:
1713474469999.png
 
Perhaps it would be better to post an example of what you want... Just guessing here....
Can't you make a plane normal to the die closing direction, project the sketch from your 45deg wall, then extrude it normally?

Here is a circle drawn on the 45deg wall, projected onto a plane normal to vertical, then extruded vertical (so that the profile is actually an oval). You can then use the "draft" function.

But maybe this isn't what you're asking for....

Sketch on wall:
View attachment 436615

Projected vertically:
View attachment 436619

With draft:
View attachment 436620

From above:
View attachment 436621
That's what I had been doing, but since I can't project the sketch with draft I end up with a distorted cutout from the original sketch once I cut with draft, because the distance from the desired sketch to the projection varies. I think that's visible in your demo with what should be a circular cut on the wall ending up as an ellipse.

EDIT: I was unable to coherently model a good example, so chose to just explain it.
 
Last edited:
I am on SW 2006 but, the features should still be the same. What I think you're looking for is the Extrusion Direction portion of the dialog box. It will either take a line or a plane / planar face as a direction.

Starting with this block and a circular sketch on the end:
1.JPG

This would be without direction control. It extrudes the hole through the block, normal to the starting sketch.
2.JPG
This extruded normal to the angled face. I selected that angled plane in the dialog and got this result.
3.JPG
This was extruded along one of the angled lines:
4.JPG
This is the same sketch, turned into a boss instead of a cut. I extruded it out from the solid body and then added a 7 degree draft angle on just the cylindrical boss with the end being the neutral plane.
5.JPG

Same geometry. All that changed between them was controlling the extrusion direction. Draft angles can be similarly controlled by selecting which face is the neutral plane.
 
I am on SW 2006 but, the features should still be the same. What I think you're looking for is the Extrusion Direction portion of the dialog box. It will either take a line or a plane / planar face as a direction.

Starting with this block and a circular sketch on the end:
View attachment 436622

This would be without direction control. It extrudes the hole through the block, normal to the starting sketch.
View attachment 436623
This extruded normal to the angled face. I selected that angled plane in the dialog and got this result.
View attachment 436624
This was extruded along one of the angled lines:
View attachment 436625
This is the same sketch, turned into a boss instead of a cut. I extruded it out from the solid body and then added a 7 degree draft angle on just the cylindrical boss with the end being the neutral plane.
View attachment 436629

Same geometry. All that changed between them was controlling the extrusion direction. Draft angles can be similarly controlled by selecting which face is the neutral plane.
That seems like exactly what I want but I can't figure out how to do that in the 2022 version. I can't find an extrusion direction option.
 
Set up a plane normal to the direction you want to cut. Open a sketch on the new normal plane. Display your desired cut shape and convert the sketch it on to the normal plane. Then you should be able to do your extruded cut. I hope i understood what you are attempting to do.
 
There are many ways to do this, some basic and some more advanced.

Make a plane as others have said, that can be done from a sketch where you draw a line at 45 from the area you want the extrude enter the die cast part, close sketch selct the plane tool pick the line and the end point and you'll get a plane perpendicular to the line, then start a sketch on that plane and extrude a cut, that way you know it is going axactly in the spot you want.

advance way would be extrude a new solid body and not murge the results, you can add fillets, draft or other features to the new body then you can use the indent tool to subract the new from the die cast.

plenty of SW vids of this online showing these tips and tricks.
 








 
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