How to create a plane on a curved surface

[contactR9VDY]

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!

[kellings]

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

[contactR9VDY]

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.

Thanks!

[kellings · Accepted solution]

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

Next click the Slice ption in the sketch palette 

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

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

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. 

Place a sketch on that plane and draw your shape 

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

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

Thanks,

Kevin

[contactR9VDY]

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

Thanks a lot!