what is the easiest way to extrude or cut from curved surfaces?

[sertanV7D8A]

Hi everyone,

I am working on this toy turtle and I want to give him a mouth, and shell texture. I was wondering what the best and quickest way to do this. 

Please let me know.

[HughesTooling]

Use Extrude and set the start to from object then select the surface as the object.

[sertanV7D8A]

That sounds really easy! I will try. I am still open to any other suggestions as well. 

[TheCADWhisperer]

Split

Presspull

[sertanV7D8A]

For some reason, none of your solutions worked for me. If you notice my object was created in sculpting form. That's why it has those split faces. So I assume there may be a connection why projections or start from the object extrusions don't work.

It takes me too long to do this. there should be an easy way. I sketch the pattern I want to extrude but, direct extrusion as the first solution suggested doesn't work. Then I project the sketch onto the surface, then it is even more useless. Then nothing works. Sketch sits on top of the curved surface, but I can't extrude, push or pull. The only thing I am pulling is my hair at this stage. Argh 

[HughesTooling · Accepted solution]

It looks like Extrude and split body don't work across edges. Split Face does work though see screencast, it shows where extrude fails when the profile crosses an edge then it shows how to create a body to use as a splitting tool.

Mark

[HughesTooling]

Just realised there's an easier way using extrude. If the sketch is outside of the body just use To Object for Extent make sure you're set to Cut and a negative offset..

Or if the Sketch is inside the object set Start to Offset Plane and set an offset that's outside your body.

Mark

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply if you can't figure it out?

[sertanV7D8A]

Okay guys, whatever you suggested I tried but nothing helps. I am very tired of this. I can't believe all these shortcomings of fusion 360. This is suppose to be a breeze.

I am attaching the file. I rolled back the history to the point where there is a sketch on top of the turtle. 

thanks

[TheCADWhisperer]

This should give you the idea....

[sertanV7D8A]

Thanks for the effort, but unfortunately that's not where I am stuck. I was able to do the extrusion in that area, but try to do the outer circle. It simply won't work. Those two you managed to extrude are part of the same face, however, when the projection falls onto a split face it simply won't work. Try and see it for yourself. 

[TheCADWhisperer]

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@sertanV7D8A wrote:

... when the projection falls onto a split face it simply won't work. Try and see it for yourself. 

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Can you post a screen capture indicating exactly where it won't work?

Also, it wouldn't make logical sense for the plates to go into the head, and I found points that were not connected.

[sertanV7D8A]

I actually managed to do it finally with using extruded bodies as the splitting face tool. I am putting the screenshot in any case so you can understand what I meant with the split face surfaces. It is such a nightmare

[sertanV7D8A]

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@TheCADWhisperer wrote:

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@sertanV7D8A wrote:

... when the projection falls onto a split face it simply won't work. Try and see it for yourself. 

---

Can you post a screen capture indicating exactly where it won't work?

Also, it wouldn't make logical sense for the plates to go into the head, and I found points that were not connected.

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I know it shouldn't go into the head, but my problem wasn't even that. I barely made it to that point. I can adjust the sketches so it avoids the head area. Thank you for your help so far. 

[HughesTooling · Accepted solution]

Here's another way to do it. Your sketch has some problems that make it hard to use to split the body so I made another body from the sketch using extrude then joined all the parts into one body to use as a tool to split the turtle body. I needed to edit your sketch a bit. My file's attached.

Mark

[sertanV7D8A]

Hi Mark,

Many thanks for the time and effort. I did exactly the same thing, but I hadn't thought about joining the extrusions, that definitely saves time. 

As you can see the tiny bits of cut out surfaces causes errors. In the beginning, I didn't notice them and I was frustrated for a while then I noticed if they are selected corrected they can be pulled. 

Thanks again. 

Sertan

[therealsamchaney]

This is a great option when it works but often times, Fusion just refuses to caluclate things. Trying this method will often result in the following error "Error: Cannot extend extrusion to object. The extrusion profile falls outside the boundary of the selected body. Select a face or plane instead, or adjust the profile so that it falls inside the boundary of the selected body." This happens even when the extrusion clearly would fall inside the boundary of the selected object.

Instead I do the slightly annoying workaround of going into the Surface workspace, clicking on the curved face and doing an Offset and set it to the depth that I want to cut. This will make a surface that's like a copy of the curved surface you want to cut but slightly inside it. Then I go back to the Solid workspace, do a normal extrude that goes through the surface as a new body, then I split that body using the offset surface as the splitting tool which will leave you with a solid you can use as a cutting tool which will cut into the curved surface the depth that you set. I know its a lot of steps but it works almost every time, whereas the more "intended" approach often fails.