Forcing an angle dimension on near parallel lines? 5

[sundevil98]

I'm trying to show a 1/2 degree angle between two lines in a drawing, but Pro/E thinks I'm trying to show the distance between where I pick on the two lines.

Is there a way to force Pro/E to show an angle dimension between lines that aren't quite parallel?

 

[dgallup]

The easiest thing is to increase the angle to say 5 degrees, make the dimension and change tha angle back.

 

[mloew]

You may wish to initially sketch the line at a more extreme angle (say ~30 deg) to get the angle dimension. You would then change the value to the 0.5 degree you need.

Best regards,

Matthew Ian Loew
"Luck is the residue of design."
Branch Rickey

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[sundevil98]

Ahhh,

Easy enough!

Thanks!

 

[mloew]

dgallup,

Just a bit quicker than I was on the "submit" button there.

Best regards,

Matthew Ian Loew
"Luck is the residue of design."
Branch Rickey

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[KimBellingrath]

Here's a little clue from my 'Think Like The Programmer' file: This applies to creating features as well as working with simplified reps - It is better to complete an operation in a gross form and then modify it after it is in existance. For difficult features - first create something obvious and then modify it to suit your demands. If it fails, you can cancel the modification. . Same goes with a big assembly; you should create a basic or empty rep to open first. Then if your attempt to open a required rep fails, at least you can cancel the operation and revert back to the 'empty' one instead of having to open the model from scratch.
Hope this helps - I've been learning since Rev 5 and the best clue is to try to think like the programmer "What does he need to know to complete this operation?" instead of "It won't let me..."

 

[onlyadrafter]

Hello,

Surely if you modelled it as an angle, using SHOW/ERASE will show the angled dimension.



maybe only a drafter
but the best user at this company!

 

[sundevil98]

The feature was a draft in a hole. I'm trying to show the angle in a cross-section view of the hole.

I tried the Show/Erase function, but it didn't show the angle the way that I needed it to be shown.

I tried changing the draft angle, but wasn't able to regenerate the model.

I've gone ahead and just created a dimension (Pro/E is still trying to give me the width of the hole) and decided to override it and put my own text in (i.e. I switched the @D to @O and wrote in 0.3').

Thanks for the help!

 

[im4cad]

You may try this too:
While dimensioning your draft, pick first the draft's edge, and then use optin "Make Line", and create your second line through a vertex of your choice, and then zoom in and click on the middle mouse button between those two lines to show the angular dimension.


im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[KimBellingrath]

NEVER! NEVER! NEVER! Create a bogus dimension in ProE!
If you're going to do things like that, just get Autocad.
One of the responsibilities of using a bi-directionally associated model/drawing system is truth in deimensioning.

 

[onlyadrafter]

Hello,

The dimension will be th truth, as long as the value isn't overridden. We do this quite a lot on complex castings where Rad and Draft dimensions do not appear in the correct position. But WE NEVER create dimensions and overwrite what has actually been modelled. Not to create dimensions would take us an eternity to have all the correct views on the drawing.



Hope this helps.

----------------------------------

maybe only a drafter
but the best user at this company!

 

[JBFJR]

Kim,
using the words "NEVER! NEVER! NEVER! Create a bogus dimension in ProE!"
Tells me you have not had the pressure of having to have prints out by 3:00 today.

They gave us this option because it is a useful tool.
And I will use autocad style dimensions to get the job done.
as onlyadrafter wrote. They are accurate just not parametric.

and besides it gives us job security

JOSE FIGUEROA JR.

 

[im4cad]

The vertex is real, is not a 2D feature, and it will regenerate for any change made, so NEVER! NEVER! NEVER doesn't make sense in this topic.
I think who gave you the star shoul take it back

im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[mloew]

I will not take the star back. Kim's theory on this subject is right on the money, although the accusation in this thread is apparently off base. The philosophy is still star-worthy, IMO.

Best regards,

Matthew Ian Loew
"Luck is the residue of design."
Branch Rickey

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips Fora.

 

[im4cad]

Taking the star back was just a joke
It's Friday people, it's weekend, we need some fun too

im4cad
Pro Design Services, Inc.

http://www.cadproe.com/pds/home.asp

 

[onlyadrafter]

Hello,

I believe therr could be a way of having thye dimension shown in the correct view, but you will need to redefine the draft and be careful as to which surface you select first. In the drawing find which is the hole in the x-section. if you have put a draft on many, then select one of the two surfaces of the first hole, or the hole in the x-section. If you then erase the shown dimension, if you haven't already erased it. Use show and erase and the dimension should appear correctly.

I'm sure I have done this on some models, but until I get back to work tomorrow, I cannot be sure.



Hope this helps.

----------------------------------

maybe only a drafter
but the best user at this company!

 

[pkgEng]

It is quite easy to dimension the angle...
Just zoom in to a point that the two lines are separated far enough apart so that you can click between them to place the dimension. If the angle is very small, then you must zoom in quite a ways.

 

[scubadude]

On the topic of adding a 'bogus' dimension...

You can always use (reference) the actual dim in the text by using the &D#... That way when the dim does change, it will change the 'bogus' dim as well...

Just a thought.

T

 

[JBFJR]

A few years back, I did this to one of my engineers on April fools day. It drove him nuts for and hour or so before I let him in on it. I just forgot how do make a truly 'BOGUS' dim.

For those who really do want to create bogus dimensions, How do you do it? I forget.

Say, I want the dim to read 18. No matter what the actual angle is. Was it something like change the actual dim to "&S"? Then type in 18 as the symbolic. Then in the drawing you would again change the shown dim to &S. The drawing would then show the 18 symbol and you could then change the nominal value to 90 and the dim would still read 18 on the print.




JOSE FIGUEROA JR.

 

[JBFJR]

sundevil98,
Has your original question been answered to your satisfaction?
I would hate to go off on this tangent and leave you guessing.

JOSE FIGUEROA JR.