I want to change one dim from driven to driver and the other from driver to driven.
This all depends on the input from the user.
Is there such a command
35068 wrote: I want to change one dim from driven to driver and the other from driver to driven.This all depends on the input from the user.Is there such a commandThanks
It is possible to do what you want inside the design table, just use logic functions on the cells of the design table range and use another two cells (outside the design table range) to define which one is driven by user input and which one is the result of a calculation.
If you don't know how to do this, post a simple sample of what you want to do (with the two dimensions, and I will create the design table to do what you want.
You can change Driven/Driving dimensions by (S)uppress/(U)nsuppressing the Relation that corresponds to that dimension. To find out what the Relation name is, right click on the dimension and select Display/Delete Relations. The prefix will be "Distance".
Mauricio, I am wondering what you mean by "to define which one is driven by user input"? Please clarify, as I have a scenario where I need to track dimensions in the Design Table that are Driven in order to harvest data about that part, however, the Design Table tends to force these Dimensions as Driving at times. Any thoughts?
Sorry if take so long to answer you.
A DRIVEN dimension is defined inside SW when that dimension will overdefine the geometry on the model (when it is not required, but when you need to use a "driven" dimension to obtain a value to be used on other calculations). When it is defined as a "driven" dimension, and included on a Design Table, the design table will read his value but it will not change it (changes on the geometry of the model will do that).
Attached is an example of a part with a Design Table using a "driven" dimension to calculate the distance between the holes. there you will see how the Driven dimension work.
This is not a good example of how to create a part like the one in the attached file, since in order to properly rebuild the part you will need to:
1.- Open design table and enter a new L dimension, and new number of FH holes.
2.- Close design table and the part will get the new L (Length) and create the new value for the "driven" dimension.
3.- Open the design table and you will see the new value for the "driven" dimension as well as the new calculated value for the distance between FH holes.
4.- Close the design table and you will see the part completelly rebuild.
As mentioned this is not the proper way to create a part like this, however it is a good way to show how you can get "driven" dimension values inside a design table and use them to calculate a value to be used in the SW geometry.
Remember, for the model to use a dimension as "driven" and the design table to not "force" it as driving dimension, the driven dimension should be one "reading" a value that it is defined not by the dimension (such as it is the case of the driving dimension on the example, which is just "reading" the distance between the centers of the circles which are "fully" defined by the geometry constrains of the sketch, if the sketch, is not fully defined and the dimension can act as driving, then the design table can force it to act as driving.
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