Tangent Dimensioning of Arcs

[Cadmanto]

This is probably a simple one, but when I dimension from an edge to the tangent of a radius or circle

it always snaps to the center.  How do I get the dimension to snap to the tangent point?

Thanks

Scott

[mflayler2 · Accepted solution]

About a minute in...

http://vimeo.com/11672625

Essentially you have to wait until the glyph changes to show tangent.

[Cadmanto]

Thanks Mark, but the firewall here prevents me from seeing the video.

What is "glyph" ?

Can you explain this in words?

[mflayler2]

Great thing about Vimeo...

In the right area of the screen I have allowed download of the video, but in case you still can't get it...

See attached image.  It will appear as you move around the arc or curvature.

[dan_inv09]

Sketch or drawing?

In a sketch you can just throw in a construction line.

In a drawing sometimes I've found that it just does not want to work. It'll look like it's going to do it and then when you click ... boom, it goes right to the center. Let it, then when you exit the dimension function you can grab the extension and drag it over to where it needs to be and it should stick.

Playing around with it just now it seems to work great for circles, but on arcs it only wants a quadrant point or maybe an end point.

You can always go the sketch route, select the view and then "Create Sketch", project what you need to construct a line then exit the sketch an put in the dimension. Then you can go back into the sketch and make your line only visible in the sketch.

[Cadmanto]

Thanks Mark.

I was able to open up the video at home.  I got it to work.

Wish you didn't have to zoom in so tight.  You would think that

the select other would toggle to this.

[Cadmanto]

Hi Dan,

This was in the sketch.  I got it to work following Marks video.

Thanks for your help.

[JimSteinmeyer]

On the other hand Dan answered my question. At least I hope I can get it to work that way.

Thank you

Jim

[Cadmanto]

Jim,

Glad this helped you as well.  I ahve not tried this in the drawing yet, but I did find it

rather difficult in the sketch though.  Should not be this hard.  I like the SW way where

you can either RC on the dimension and change the location, or just drag the end point

to the desired location.

[JDMather]

For beginners reading this thread - just a note: machinist hate this type of dimension as it is very difficult to hold tolerances in the manufacturing environment (read - increase cost).  Use only if a critical dimension - otherwise dimension to centerpoint locations of arcs.

[JimSteinmeyer]

Unless of course you have a boss who insists that the center of an arc on the edge of a part is an imiganary location with no way for the fab department to measuer to it.

There really are times where dimensioning to the edge of an arc makes things more user friendly. While machinests like to the hole center most fab departments have less technical employees and tape measures at best. for them to locate the hole center takes a calibrated eyeball and good guessing. I wish inventor would make some of these options much easier to do, or at least clearer to figure out how to do.

Jim

[jeanchile]

The steel fabrication shops we work with prefer the tangent dimensions (looser tolerances) and some of the machine shops we work with have asked for it as well. Most of the machine shops that we work with prefer the centers though.

[Cadmanto]

Like Jim I have seen both.  I totally think this depends on the shop and the operator as well as the application.

[ronald_plesh]

What if it never changes?  I cannot believe how much trouble I have with this function, I feel like an idiot.

[dan_inv09]

I don't know if you read any more of the thread but as was said, it seems to be more forgiving when you are modifying a placed dimension then when you are placing it.

So if you place the dimension wherever it wants to go and then drag it to where you want it you may have better luck.

[Curtis_Waguespack]

---

@ronald_plesh wrote:

What if it never changes?  I cannot believe how much trouble I have with this function, I feel like an idiot.

---

Hi ronald_plesh,

It's not something to do with the size of the arc / circle again is it?

see link:

http://forums.autodesk.com/t5/inventor-forum/help-placing-a-dimension-from-a-line-to-the-tangent-of-...

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[ronald_plesh]

Nope, the circle is only R14.563.  It is near a section view though.  I can dimension from the edge to the intersection of the section line and the curve.  So I think its all good.

Thanks again.

[ronald_plesh]

The trouble is this does not always work.  The glyph NEVER changes.  It just switches to a selection box.  Look at the vide.

Now what do I do?  That is in a sketch in Inventor 2016.

 http://autode.sk/2hZNRvm

[dan_inv09]

I've been playing around with it and it seems to be a fixed distance - about half a millimeter. When I tried to get my scale the same as yours I could not get it to switch, I was like, "It worked when I just threw up a circle!?!" but then I picked the line and zoomed in to grab the circle and it appeared just for a second. Then I zoomed in some more and was able to get it a little further away. Then I thought, "I'll throw down a line about where I see it." and when I zoomed in more it appeared about at the line, and when I zoomed out - if I could still make out that line I could get the tangent, when that line was indistinguishable from the center-line I couldn't. Zoom in close enough and tangent is all you'll get.

So pick your line then use your mouse wheel (or space-mouse/ball etc.) to zoom in on the circle.

And post to the IdeaStation to tell them to make it not an absolute dimension - it should scale so that you can do it with big circles. (I guess just 29 inches in diameter counts as a big circle (and Curtis deserves a Kudo).)

[dan_inv09]

Remember how I said it's a fixed distance?

I just came across a new wrinkle: I'm trying to dimension from center to center of circles that are about 1 mm in diameter ... and I can't! It always dimensions the tangent if I try to just grab the circle, all the way around. I have to specifically go to the center-point if I want to dimension to the center. (Yeah, okay, that's not really a huge deal. Unless maybe you were working on really tiny stuff, then it might be more trouble. But I'm used to the larger scale behavior and it's annoying that things are different just because it's zoomed in.)

Did anyone ever get around to making an Idea to change this?