Sketch lines not recognized for profile

[Noah_Katz]

As seen in the screencast, the 11.5 dia circle isn't recognized for the profile whether it's projected or explicitly drawn.

What am I doing wrong?

[etfrench]

Most likely it's not the top surface.  Turn visibility off on all items except the sketch containing the circle.  Once the circle has been selected, you can turn visibility back on if needed for the extrusion operation (join, cut, extrude to, etc.).

[Noah_Katz]

I didn't think of that, but actually it is the top surface

[etfrench]

Why didn't you extrude it after you had selected it and opened the extrude dialog?

[HughesTooling]

It looks like you have 2 profiles at that level and Fusion's picking the other one first. Click and hold the mouse button down until you get the selection menu then pick the one you want.

[Noah_Katz]

> Why didn't you extrude it after you had selected it and opened the extrude dialog?

Because I want the circle with the cutouts.

[HughesTooling]

The cutouts are in a different sketch, you need to project them into the sketch with the circle.

Mark

[Noah_Katz]

Ah, I assumed that edges from the face I'm sketching on are automatically  included, like my previous CAD.

Wait, that's true, as one of the profiles does include the cutouts.

I activated the part I'm sketching on and tried it again, with exactly the same result, as shown in the screencast.

Gotta go now, will check back in several hours, or maybe I can answer w/the app.

[HughesTooling]

In your first screencast is there a chance you had a sketch visible when you create the new sketch?

If you have a sketch still visible on top of the body when you pick you might select the sketch and you don't seem to get autoproject from a sketch.

Mark

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[Noah_Katz]

> Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

Apparently not; the only types shown for export are IGES, STEP, SAT, and SMT.

[etfrench]

Archive File (*.f3d) should be available.  Save the file locally, then attach to forum thread.

[Noah_Katz]

Ah, I missed the message that popped up at the lower right saying I had to break all links (why the heck don't they persist long enough to notice/read them?).

[Noah_Katz]

Just noticed that I had two sketches on the part; I deleted both, tried again, and it worked.

I backed up and checked the first sketch, and it had nothing in it, so not sure why that would matter.

Just for kicks I deleted the new component and did everything I did the first time, and it worked.

Could it have something to do with deleting the last link and/or exporting?

When I first deleted the link I had tried it again and I thought it worked, so I backed up and did it again during a screencast, but then it didn't work again.

[HughesTooling]

If you had another sketch visible and picked the face it was on the sketch will be used as the plane for the new sketch not the surface and you will not get any edges projected from the surface. Was the sketch you deleted really empty, a sketch created on a face will have all the edges of the face projected in when it's created. 

Mark

[HughesTooling · Accepted solution]

Just downloaded your file and you have 3 sketches visible the none of the sketches are empty or is there another one?

Screencast shows the curves in the sketches.

Mark

[Noah_Katz]

Mark, that's it, thanks!

I didn't realize that all visible (at least according to their light bulbs; see below) sketches were in play; I thought it was only the currently active one.

But I guess as soon as Extrude etc. is selected, the sketch is closed and any visible sketch is fair game.

Mot plt was the very first part I made, and of course neglected to create a new component first, so the sketch is stuck belonging to the base component.

It doesn't help that Sketch 16 is only visible when the cursor is moved over it; any idea why that is?

[HughesTooling]

As a quick test try this, create a body can be just a cube. Create a new sketch and select a face, without drawing anything stop the sketch and hide the body. You should see a shaded profile and if you move the mouse over the edges the edge lines will highlight. I don't like auto project and have turned it off in preferences if I want all the edge curves I press P and select the face but I like to keep my sketches neat so generally I just project in lines and points I need.

Mark

[Noah_Katz]

Ah ok.

The part geometry is actually in the first sketch so not sure why Sketch 16 is even there; probably just newbie klutzing around.

>  I don't like auto project and have turned it off in preferences if I want all the edge curves I press P and select the face but I like to keep my sketches neat so generally I just project in lines and points I need.

Good to know.

Is there a way to project connected edges, like the ones defining the cutouts?

I tried double-clicking and ctl but that didn't do it.