Project Sketch onto curved surface then extrude?

[steveripplingerjr]

I am trying to project a scketched pattern on to a curved surface then extrude, I have not problems doing this on a 2d surface. 

I for the life of me cannot get it to work.

I am creating my 3d body, I then create an offset plane. Create sketch pattern, close sketch, create new sketch, Project to faces along vector. Then I get pink lines and it takes forever. I cannot extrude my pink line pattern on the surface? 

[taylor.stein]

Hi Steve,

Great question! As far as I'm aware, this projected curve onto a non-planar surface cannot be extruded using the Extrude command within the Model workspace. I have found that you are able to extrude the projected curve in the patch workspace. You might be able to pair this with some patches, stitching them all together to create a solid. This is simply a workaround that might work for you - depending on what you're trying to create. 

Can you share what it is you're trying to create?

Let me know if you have any other questions, or if you need further explanation!

Taylor Stein

Fusion 360 Evangelist

[jeff_strater · Accepted solution]

Another option is to use Split Face (select the proejcted curve as the split tool) and Press/Pull (select the split face):

Jeff

[steveripplingerjr]

That works. It wont be fast but it will work.

[Anonymous]

Thank You!

As a new user of Fusion 360 I have been struggling to work out how to do several things and I just noticed your post that seems to be the solution to my task in hand.

However I've got stuck on the next step - I need to repeat the feature all round the cylinder (an a cone on the next item). I thought this would be easy using a circular pattern but I have failed.

The first image attached (pattern.jpg) shows the screen just before hitting the OK button - it seems fine to me.

The other image (error.jpg) shows the message after hitting the OK button.

Do you have any ideas what I may be doing wrong?

Regards,

Andrew Nummelin

[HughesTooling]

Depending on how you made the part but it might work better with pattern feature, third icon from left then select the feature\features from the timeline. If that doesn't work can you share the design. To export right click the top node in the browser and select export and save as an F3D.

Mark

[Anonymous]

Thanks for the hints. I'll give these a try tomorrow on the real target (because you have already seen it) rather than on a simple example piece: it will be a slow process as I have to first calculate all the design dimensions.

Regards,

Andrew Nummelin

[Anonymous]

Mark,

 Two files are attached, the first to show the types of thing I am trying to draw (for 3D printing of a small scale model). The second is the Fusion file showing how far I managed to come.

I sketched the outline of the flute (0.5mm wide at the bottom and 0.42mm at the top) and used "modify, split face" command to transfer the outline onto the conical section.

I then used "modify, press puill" to push the flute outline 0.25mm into the cone.

The flute was finished by using "modify, fillet" (0.2mm radius) on the outline of the bottom of the flute. Not pefect, but fine for a small model.

I then selected on the time line the operations to create the flute, selected "create, pattern, circular pattern". In the "circular pattern" dialog box I selected the axis of the cone, changed the quantity to 24 and left the other options unchanged, and clicked on OK. The operation failed.  I tried several other options but none worked.

Have I missed something simple, or would a totally different approach have been more appropriate?

Regards,

Andrew Nummelin

[HughesTooling]

I can't get it to work using the split face method but here's another way using revolve.

Project the cylindrical part to the plane running through the centre of the model, then draw a construction line between the points of the 2 lines. Then construct the cross section of the flute.

Then make a revolve cut and a feature pattern.

File's attached.

Mark

[HughesTooling]

Here's an other go, I noticed the flutes need to be tapered, so I modified the sketch so the diameter can be different at each end.

Mark

[Anonymous]

Mark,

          VERY many thanks - exactly what I needed. There's clearly lots to learn about this program!

Regards,

Andrew Nummelin