How do I force dimension to show 45 deg instead of 135 or 225?

[sschulteH6WZ3]

Why will inventor not give the option to give an acute angle dimension instead of an obtuse angle dimension? I want to show 45 degrees instead of 135 on a detail drawing. No matter what I do it will only show 135 or its opposite 225. Using Inventor 18.

[mcgyvr]

You can't just drag the number over there and it swaps..

Thats how it works for me very easily....

Can you post your idw file?

Something does look "skewed" though in your drawing.. Why is that 3/8" dimension not parallel to the body? Why are there 2 extension lines not parallel on the other side of the angle dimension away from the 135 deg text?

[sschulteH6WZ3]

No it does not swap automatically. What looks skewed is actually a curved surface part of a 18' 8-1/4" ID ring made of structural c channel.

[mcgyvr]

Can you post the idw file? (and maybe the ipt/iams)

As it seems this is model specific so.... 

[kelly.young]

@sschulteH6WZ3 I would play around with the angle dimension options and see what you can find out.

The screencast shows a few ways the dimension can get locked to one side, but that is typically after you force it to be that way. If you just add a new dimension it should be able to swap sides easily.

Hope that helps!

Please select the Accept as Solution button if a post solves your issue or answers your question.

[sschulteH6WZ3]

Kelly, mine wont do that. No mater where I move the mouse it will not show any thing other than the obtuse dimension. As a workaround I have to exit out of the command and then right click, options and then click use quadrant each and every time I put a angle on a drawing. Once I have done that then I can show the dimension the way it should be. Then next angle I have do it all over again what should be one step is 4 steps. Its just one big time suck. For the life of me I don't know why it wont let me do it automatically as you show in your video. 

[mcgyvr]

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@sschulteH6WZ3 wrote:

Kelly, mine wont do that. No mater where I move the mouse it will not show any thing other than the obtuse dimension. As a workaround I have to exit out of the command and then right click, options and then click use quadrant each and every **** time I put a angle on a drawing. Once I have done that then I can show the dimension the way it should be. Then next angle I have do it all over again what should be one step is 4 steps. Its just one big time suck. For the life of me I don't know why it wont let me do it automatically as you show in your video. 

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Its a data specific issue...

Can you post your dataset (pack and go or whatever) so someone can see what specifically you are working with there?

Post your idw/ipt and if thats an assembly the iam file too.. 

[kelly.young]

@sschulteH6WZ3 My guess is that the view of the part is not normal to the drawing plane.

If the part is askew it won't pull a normal angle dimension which is why you have to use the 3 point angle.

If you can use the Custom View Orientation and Look At the face you want to dimension it should pull dimensions easier.

If you can post your parts maybe we can investigate and find a better way.

Please select the Accept as Solution button if a post solves your issue or answers your question.

[sschulteH6WZ3]

Unfortunately I am working on a customers print package and they were very specific about not sharing drawings or models with out their permission. Let me see if I make a new independent drawing if it does the same thing.

[JDMather]

If all else fails,

select the view

click S on the keyboard

Project Geometry appropriate geometry

sketch your own extension lines and constrain as appropriate

Finish Sketch

you should now have two angled lines that you can dimension.

or....

create a dummy part and drawing that exhibits the same behavior as your proprietary files and attach the dummy set here.

Someone will create a Screencast video.

[okaleja · Accepted solution]

Hi,

Please make sure you have Dimension Style correctly setup. There is forward create option which controls this behavior. Notice the option on the screenshot below.

Hope this helps,

Oto Kaleja

Autodesk