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How to create a plane on a curved surface

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Message 1 of 5
contactR9VDY
229 Views, 4 Replies

How to create a plane on a curved surface

Hi,

I've been trying to design a funnel for a coffee grinder. It's going rather well given my knowledge of fusion360. Unfortunately, I've stuck and can't really find answers for this particular problem.

 

So, I'd like to make a lid that is 30mm wide and 80mm long on top of a funnel. It should cut through the upper layer of the funnel to provide a cleaning hole for the ground coffee.

 

Basically I want to cut out a rectangular hole on top of a curved funnel but I can't figure out how to tilt the plane.

 

Any idea would be appreciated!

Thanks!

4 REPLIES 4
Message 2 of 5
kellings
in reply to: contactR9VDY

Hi @contactR9VDY Sorry, I'm not entirely following what part you a specifically referring to. On truly curved surfaces, you can use the tangent plane. From the construct menu, select Tangent plane and then click the face of the curve.

 

You have some areas on your part that look to be curved, but they are more complex and are splined surfaces instead of a curve. So there is a different workflow to find that plane. 

 

Even if you did a screen shot and drew on it what you are trying to accomplish, that would be helpful.

 

Thanks,

 

Kevin

Kevin Ellingson
Technical Specialist

If my post resolves your issue, please click the Accept Solution button.
Message 3 of 5
contactR9VDY
in reply to: kellings

Hi,

Thanks for taking the time helping me out!

Yes, the problem is that the top of the part isn't really a curved surface but created using "loft" so I can't find a curve to create a plane on it.

I've created a screenshot. Where the red rectangle is drawn I'd like to make a lid. lid.jpg

 

Thanks!

Message 4 of 5
kellings
in reply to: contactR9VDY

Hi @contactR9VDY Thank you so much for that image. It was very helpful for me. That was the surface I was referring to as the more complex one that you can't just place a tangent plane. Here is how I went about this. 

 

Create a sketch on the plane as shown

SelectPlane.png

 

Next click the Slice ption in the sketch palette 

SketchSlice.png

 

From the Create menu, choose Project / Include --> Intersect. I then selected these points shown in magenta with the red arrows pointing at them

ProjectPoints.png

 

Next draw a line from point to point. Then you can finish your sketch. 

SketchLine.png

 

Switch to the Surface tab and extrude that line using the symmetric direction option. This will create a surface body that will be planar. You can extrude it as much or as little as you like. This is just going to be used as a sketching plane. 

SurfaceCreate.png

 

Place a sketch on that plane and draw your shape 

SketchCut.png

 

Then you can extrude your shape. Note that you may have to make sure the Operation Type is set to cut

ExtrudeCut.png

 

Let me know how that part works out for you and if you have any questions. 

 

Thanks,


Kevin

 

Kevin Ellingson
Technical Specialist

If my post resolves your issue, please click the Accept Solution button.
Message 5 of 5
contactR9VDY
in reply to: contactR9VDY

That's amazing! That was exactly what I was looking for!

Thanks a lot!

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