cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Community Tip - You can subscribe to a forum, label or individual post and receive email notifications when someone posts a new topic or reply. Learn more! X

How do I force a dimension type in sketcher? Creo 2.0.

rbast
1-Newbie

How do I force a dimension type in sketcher? Creo 2.0.


I have a slot that is .6° off the bottom of the part.  I have created a construction line between the ceter points of the two arcs.  When I try to dimension an specific angle it will only pick the end points of the line.  In Catia (my main program) I can choose a dimension type like angle before making the dimension and the program creates an angle dimension.  I can't seem to get creo to behave the way I would like it to.  That is forcing the dimension creator to limit it'self to an angle dimension.  How do I accomplish this task? 
.
I am converting parts from Catia into Creo and need to match the dimensioning scheme.  So an angle dimensoin is required.


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.
1 ACCEPTED SOLUTION

Accepted Solutions
Chris3
20-Turquoise
(To:rbast)

By default minimum_angle_dimension is set to 1. Try adding this to your config.pro:

minimum_angle_dimension .1

Alternatively if you don't know what a config.pro is, go to file -> options -> configuration editor -> add

View solution in original post

4 REPLIES 4
Chris3
20-Turquoise
(To:rbast)

By default minimum_angle_dimension is set to 1. Try adding this to your config.pro:

minimum_angle_dimension .1

Alternatively if you don't know what a config.pro is, go to file -> options -> configuration editor -> add

rbast
1-Newbie
(To:Chris3)

That is seeming to do the trick.  When I entered it it was set at 1.0.  Changing it to 0.1 is allowing the angle dimension to work.  Thanks.

Tmetcalf
Emeritus
(To:rbast)

Good day Richard,

Glad you were able to get back on track.  If Richard's solution fixed your issue, would you please mark it as a "Correct Answer?"  This helps all following the discussion know the solution.

Best,

Toby

Another trick to work around this is to exaggerate your sketches - so even though the final angle is 0.6°, draw it (by eye) at more like 30°, create the dimension and then change the value.

When creating features around an angled plane as a centreline, I often create it at a relatively large angle (usually 23°, for no particular reason) to the default plane, just so that it's completely clear in the sketch which plane I'm selecting as a reference, and I don't select a default plane by accident.  Then when I'm done, I change the angle of the plane to its 'correct' value, such as 5°.

Top Tags