Check if a parameter is within range

[CAD_user]

Is there a option in creo to check if a certain parameter or measure is within a range?

Example:

Imagine that i have in my design, a spring, that it's maximum stroke is 30mm. This spring is correctly dimensioned while the stroke is below 30mm. But if in a special condition i need to put 50mm of stroke, creo sends me an alert that the stroke of the spring, is higher than its range.

I have an example from SolidEdge, that represents a similar situation

https://www.youtube.com/watch?v=1lA0bcT5BJU

[DaveMartin]

Here is how I've seen it done:

Create a string parameter called something like ERROR_MSG with an initial value of "".

In the Relations dialog box, write an IF-THEN-ELSE relation that evaluates the value of the stroke, and depending on the result, assigns a value to ERROR_MSG such as "STROKE IS HIGHER THAN RANGE."

Then create a 3D Annotation using Flat To Screen so that the value of ERROR_MSG appears in the Graphics Area.

You can also create a relation like STROKE <= 50 so that violations of the condition are reported in the Message Area, but that is not as obvious.

[Ketan_Lalcheta]

If you are not willing to go with Relation, You can use restricted parameter.

http://support.ptc.com/help/creo/creo_optm/usascii/index.html#page/optm/options_modeler/fund_seven_sub/about_Restricted_Value_Parameters.html

HIH

Ketan

[TomD.inPDX]

Dave's solution is what I would go with using "IF" statements that defaults to within range if a non-valid value is entered.  Nice to see I can warn a user with Dave's technique.

Funny thing is that we rarely see the relations function as a programming tool.

However, the method I might go to for assemblies is mechanism constraints.  These have a lot of built-in options including limits and regeneration defaults.

This is similar in function to the SW under the advanced assembly constraints.

However, the video is set up for kind of analysis function.  I'm sure this is available in Creo somewhere but may require additional modules.  There are some light versions of various analysis tools in core Creo.  I am only familiar with Simulate lite for simple FEM functions.