topic Re: How to extrude a 3D Sketch in Inventor Forum

How to extrude a 3D Sketch

BjarneVanBuggenhout — Thu, 08 Nov 2018 16:40:16 GMT

I have got a 3D sketch into my cilinder...

Now is there a way to cut away to upperside of the cilinder, so i have the spline waves cut out?

Re: How to extrude a 3D Sketch

Cadmanto — Thu, 08 Nov 2018 16:44:02 GMT

It looks to me like you could create a surface using the 3D sketch, then create a sketch above them and extrude cut to these surfaces.

Hope that makes sense.

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Re: How to extrude a 3D Sketch

jtylerbc — Thu, 08 Nov 2018 17:21:23 GMT

Another option might be to create the surface as @Cadmanto described, but then use the Sculpt command and select the surface as the cutting tool, instead of using an extruded cut.

This would eliminate the need for the extra sketch he mentioned, while giving the same end result.

Re: How to extrude a 3D Sketch

leowarren34 — Thu, 08 Nov 2018 19:50:27 GMT

I believe that if it is uniform than create a solid and split it along the spline using it as a path.

Re: How to extrude a 3D Sketch

johnsonshiue — Thu, 08 Nov 2018 22:44:12 GMT

Hi! Adding to Scott's and John's comments, you can also use Rule Surface command and select a direction to "extrude." Result is a surface based on the 3D profile sweeping along the direction in a given distance.

Many thanks!

Re: How to extrude a 3D Sketch

Anonymous — Fri, 09 Nov 2018 00:39:37 GMT

Three methods come to my mind right now.

All start by creating a surface from the 3D sketch with "Patch".

1: extrude from a 2D sketch below, extent "To" -> select surface... or if an existing solid goes through, do the same with extruded cut

2: If an existing solid goes through, use "Split", pick "Trim Solid", then select the face as "Split Tool".
3: existing solid below or above: Click "Replace Face", select your flat cylinder face as "Existing Face", then the surface as "New Face".

Re: How to extrude a 3D Sketch

BjarneVanBuggenhout — Fri, 09 Nov 2018 15:18:05 GMT

This was very helpfull,

but I didn't got it quite right...

I want to make te cut "straight", like this:

If i want to cut to this plane, I've get a failure:

Re: How to extrude a 3D Sketch

johnsonshiue — Fri, 09 Nov 2018 19:41:14 GMT

Hi! The error might be due to the surface being smaller than the solid. Try using Extend command to extend the surface further (inner and outer loops). Make sure the surface covers the solid body.

Many thanks!

Re: How to extrude a 3D Sketch

BjarneVanBuggenhout — Mon, 12 Nov 2018 11:16:40 GMT

still the same error...

Re: How to extrude a 3D Sketch

BjarneVanBuggenhout — Mon, 12 Nov 2018 11:26:13 GMT

It worked, I used the split command instead of the extrude command!

Thanks for the help!

Kind regards,

Bjarne