Unable to create threads on a component made with the revolve operation

[Anonymous]

Hello, I have been trying to make a thread on an internal and an external face of an object I modeled using a revolve operation. I've tried several times and in different ways but have been unable to accomplish what I need. I hereby attach a screenshot of the object and the selection of the internal face I'm trying to thread.

Thank you for your time,

Yolanda

[HughesTooling]

You can create threads on revolves OK so it's something to do with your design. I'd guess it's the smaller diameter behind the thread that's the problem, it need to be smaller than the core diameter of the thread or it'll fail.

You can see in this image it works ok but if I make the highlighted hole bigger than the core of the thread it fails.

Mark

[HughesTooling]

@Anonymous In the future can you use the Photo option on the tool bar to embed images please.

Mark

[HughesTooling]

@Anonymous Here's an idea for a workaround. Split the body, add the thread then combine.

Mark

[Anonymous]

Hello, thank you so much for you response. Unfortunately, that is not it. I can only select (highlight) the face before clicking on the Thread operation. Once I do that, it doesn’t let me select the faces. I’ve tried changing the diameter of the thread but it doesn’t work. The core diameter is 90mm.

What do you mean by splitting the piece?

Thank you,
Yolanda

[Anonymous]

I just saw the video about the split idea, let me try it and get back to you!

Yolanda

[Anonymous]

Hello, I did the split just like the video and wasn't able to create the threads 😕

Any other ideas?

[HughesTooling]

Is it possible to share the design here? If you don't mind sharing it, Export as a f3d and attach.

From your description that you can't select the face it sounds like it's not a cylindrical surface. If you use the inspect tool does it give you a radius and diameter if you select that face?

Mark

[Anonymous]

Yes, it gives the the length as well as diameter and radius. The internal face I am trying to thread is the highlighted one in the past image, and the external face is just the one on the other end.

Here's the file 🙂

Thank you on advance!

Yols

[HughesTooling]

Actually if you select the surface, not the edge you don't get any info about diameter\radius.

The quick answer to your problem is the line in sketch2 is not horizontal so the part is a very shallow cone. The bigger problem you have is neither of your first 2 sketches are fully constrained so the whole design is build on shaky foundations, you need to anchor the sketch to the sketch origin. At the moment your first sketch is just floating and any modification is unpredictable.

Mark

[Anonymous]

Thank you so much Mark !!

I saw that contraints could be a problem on other posts, but when I went back and tried to fix it it said it was over constrained. But I'm gonna check the sketch again and work on what you are talking about. Any tips for constraining this sketch in particular?

Thank you,

Yols

[HughesTooling · Accepted solution]

@Anonymous I found your first sketch a bit puzzling, I don't know if you had a plan that's not obvious or you just don't have experience with technical drawing. Any way here's a quick screencast demonstrating how I'd construct a sketch for a revolved part. A couple of things to note, I draw the rotation axis first making sure it's horizontal. Then when adding dimension needed for the diameter if you select the axis line first then right click you can specify a diameter rather than radius. When the sketch is fully constrained note all lines are white and changes to dimensions have a predictable result.

Mark

[Anonymous]

It is probably that I'm very rusty on technical drawings, I would normally use SolidWorks and I always managed to constraint the drawings but when I try to constrain the sketches here I can't. Gonna check the video and fix it and I'll get back to you. Thank you very much Mark..

Yols

[HughesTooling · Accepted solution]

Yols, an odd problem in your first sketch is the white point you have near the sketch origin, you have several dimensions anchored to it but it is not actually a fixed point. If you add a coincident constraint to the origin several lines are then fully constrained. Here's a short screencast using your design. I got stuck trying to constrain the internal ribs, I'll leave that up to you to figure out, you might want to delete some dimensions, add parallel and horizontal\vertical constraints then add back the angle dimensions.

Mark

[TrippyLighting · Accepted solution]

Are you familiar with Fusion 360's R.U.L.E #1 and #2 ?

[TrippyLighting · Accepted solution]

Overconstrining can be a problem, but under constraining is usually more "dangerous.

In genereal "something" in a sketch has to be referenced to the sketch origin, which I've circled in the screenshot below, or to another sketch element that was projected form an edge, face, body or other sketch element.

I'f you've got experience with Solid Works then you already know how that works. The constraint system in Fuiosn 360 is still a little shall but it is getting better. I personally avoid patterning and mirroring in sketches and rarely use the equal constraint. 

Horizontal/Vertial, Perpendicular and Midpoint r eat ones I use mostly.

Part of that is also completely dimensioning a sketch.

If a sketch gets too complicated, it often helps creating more than one sketch.

[Anonymous]

I fixed the sketches and constraints, thank you Mark and Peter for your help!!

Here's a screenshot of the constraint sketch and successful threads. 

Thank you very much !!!!!!

Yols

[HughesTooling]

Just need to teach you to use the photo option on the toolbar to embed images now. Job looks good.

Mark 

[Anonymous]

I just had this problem. I fixed it by deleting the revolve and re adding it.