Inventor inverts angular measurments in drawings

[Anonymous]

I have encountered a frustrateing problem with angular measurements.

In a drawing of, for example a gear, I want to place an angular measurment from one kog to another with respect to the center line.

I use dimension, click on one point on the first kog, then on the center point, and latly on a coresponding poin on the second point. Inventor then produces a prewiev measurement to be placed, it looks normal (1st pic). Once placed, it changes the measurment to the inverse and makes it huge (2nd pic). I can rearange the measurement but never invert it (3rd pic). Why is this happening and what can I do about it?

[-niels-]

Not sure if this helps, but if you right-click on the angle dimension and go to "options -> use quadrant" are you then able to change it to the angle you want?

[Anonymous]

Thank you, that change the behaviour but its still inverted and wount allow me to modify it to look at is did when I placed it.

[-niels-]

Under the same right-click options there is also an option for "opposite angle", does that change it?

[Anonymous]

No, tried all the options in different combinations.

[-niels-]

Not sure why it's happening, but if those options don't help you could always make a sketch on the view and make some construction lines to attach the dimension to instead of using points...

[Anonymous]

That worked but its a bit of a work around. Hope I can figure out why it does that.

[Anonymous]

Attaching the files that I used in the example

[bobvdd]

Can you recreate the views? I am not succesful in creating ANY angular dimension with the 3 picks that you explained on the existing view.

When I recreate the view , the angular dimension can be created without problems. BTW I am on 2016.

[-niels-]

@bobvdd i made a screencast with @Anonymous's files so you can see how to do the 3 picks.

I'm also on 2016 and couldn't recreate the behavior.

(to other readers, the original files are 2015 format)

[Anonymous]

This is very odd. I couldn't create any angular measurments either once the drawing was closed and reopened.

After deleting the wiev and inserting a new one I could create angular measurments. Most didnt invert but they were expanded well outside the sheet once I hit "ok". Some did invert after showing up normaly in the prewiev.

After a while of experimenting ALL measurements started to apear inverted and expanded again.

I teach and some CAD is part of my clases, some of my students experiance the same problem. They have been installing from their own downloads. 

Im willing to accept that it might be something Im doing but I dont understand how that would result in the change in behaviour the file is showing.

[Anonymous]

Here is what it looks like on my laptop.

[bobvdd]

Thanks Niels and Peter. I now see that the center of the gear is inferred by touching the circumference.

I went back to 2015 Sp1 but I cannot reproduce the problem in 2015.
The angular dimension gets created correctly with the smallest angle and does not jump away from the center.

But I have seen another weird thing on the existing view:
I cannot create an angular dimension between following two centerlines (which would otherwise be my preferred method to dimension this situation). But once again when I recreate the view, the dimensioning to the centerlines starts working. 

Hence I am thinking that there is a small precision problem with the existing view (maybe it is not entirely parallel to the drawing sheet ?!).

How was the view created?

[Anonymous]

I got similar results. I could not place angular measurments in the original drawing but once I recreated the wiev it workd. Angular measurments still behaved in the way I previously described.

Both wievs were created using "place wiev">"base">"top". The part was created using the standard planes.

Still, using center lines worked out fine once I recreated the wiev wich at least gives me a relibable way to place wievs. 

I did try creating a drawing using "current" on a heavily tilted part and it worked just as the others.

[okaleja]

Hi,

I noticed that for whatever reason you have the General Dimension Type set to True on the view. That's not correct. True dimensions don't support centerlines and center marks. You should change that setting to Projected (via RMB menu on the view).

Hope this helps,

Oto Kaleja

Autodesk

[Anonymous]

I get the same behaviour both with "true" and "projected". I didnt chose "true", it was the default for whatever reason. I did some reasearch and my model is created in the standard planes which, as far as I understand, would mean that true should work fine.

Im not sure what you mean by "True dimensions don't support centerlines and center marks." I used center mark to create the borked up angeles as well as the few normal ones.

[okaleja]

General Dimension Type setting does not affect already placed dimensions. It is used by the Dimension command only when new dimension is created. When you have this setting set to True, you are not able to select (dimension to) centerlines and center marks. It is possible there is some other selectable geometry, e.g. center mark and arc center overlapping. So make sure you select the right item.

Oto Kaleja

Autodesk