Dimensioning to tube or pipe "center line radius" (CLR)

[mattCZZUT]

Four year old thread here: https://forums.autodesk.com/t5/fusion-360-design-validate/how-to-dimension-to-a-radius-centreline/td...

Two year old archived community post here: https://forums.autodesk.com/t5/fusion-360-ideastation-archived/centerlines-for-curves-in-drawings/id...

I can't see this on the roadmap as per the community post.....so.....

1. Anyone know if its is happening? Or,

2. Anyone know a work around to dimension to a tube CLR? Sorta essential for tube bending as dies are all measured to the CLR.

There was one suggested workaround I've pasted below, but I can't figure how to make this work, so any suggestions would be appreciated....

"If you create the solid model using a 2D Scetch, for example lofting a tube or similar on a path, you can right click and create the sketch as normal construction, and/or when you create drawing make sure that the browser is expanded to show sketches and turn the sketch lightbulb on, you should then have a CL on the tube, rid or wire with a curve."

I haven't been able to figure this part out: "....you can right click and create the sketch as normal construction...."

TIA

[ClintBrown3D]

Hi @mattCZZUT 

Welcome to the forum!

You can turn on the sketch that was used to create the Pipe/Sweep feature in the drawing, this is displayed as centre line geometry that you can then add dimensions to.

I hope this is helpful

[mattCZZUT]

Hey Clint, 

Thanks for helping me out. 

I can't make this work as you've shown me. Probably because I have made a mess of the underlying sketch. Its not quite a 3D sketch but its on three planes.  Likely noob mistake. 

Even with the sketch turned on in the drawing its not visible (toggling Sketch 7 makes no difference to the drawing). Not sure why Sketch 2 is greyed out. Didn't have any luck finding a tutorial on YouTube or in the forums. 

The constraints are: the two uprights must be on 260mm centres as per the drawing, and the tube is dia 32mm and the bender die I've got on hand to make this part is 4.5" center line radius. The rest I'm just messing around trying to make the drawing work as a learning exercise.

If I have overlooked a lesson somewhere in the archives, I'd appreciate being pointed in the right direction.

Thanks,

Matt 

[HughesTooling]

Can you share your design? Export the 2d drawing as an fz3 file and it'll include the 3d model.

One note is be careful dimensioning the arc below, because it's on an angled plane the radius will not be correct looking down in this view, actually it will probably be a spline or ellipse you will not be able to dimension. Really you need a view aligned with the angled plane to dimension correctly.

[mattCZZUT]

Hi Mark, yeah true, that 20 degree plane will need its own view to correctly dimension it.

I'm still learning, especially the pipe function, so I've probably constructed the sketch wrong to start with, so if you see any obvious problems I'd be grateful for any pointers.

My "File/Export" option was greyed out in the drawing, but I could export from the part design. However I have no option for "FZ3" export as per your instructions, so I've used F3D. 

Appreciate you offering to help Mark.

Cheers

Matt

[HughesTooling]

I've come up with a reasonably robust 3d model but it's not fun working with 3d sketches in Fusion. Someone else might come up with something better.

Basically what I've done is make your first sketch 2d, created an offset plane and projected from the first. Also for parametric models try and avoid the primitive shapes. Not sure why you had the Box so I just deleted it.

Here are the 3 sketches and offset plane used to drive the part.

Next I created another sketch and projected the curves using Project Include 3D Geometry. I found the projection of the angled arc was not reliable if you edited the sizes.

And here's a screencast adding the lines and fillets, make sure you have 3d sketch enabled. For the first arc I click the first point then click and drag to the second point using the line tool. After adding the fillets some constraints are removed and need adding back. I think if you create an aligned view in your 2d drawing, sketch7 should now give a centre line. The way you had it, your angled sketch had an ellipse because you projected from the XY plane to your angled plane. File's attached

Mark

[HughesTooling]

Just experimenting with the 2d drawing and I noticed 3d sketches are greyed out and can't be used. What you'll need to do is project the 3d sketch into another sketch. For the angled part here's a screencast, I create a centre line as a helper while creating a section view then move the section line to give an aligned view with the sketch now visible as it's aligned with this view.

Mark

[mattCZZUT]

Hey Mark, thankyou very much for the screencasts. I need to spend some time to digest, follow and understand what you've done. I'll revert if I have any intelligent questions!