I have a parameterization table with different values for a diameter: standard, maximum and minimum.
I would like to be able to assign the "standard" value to a parameter that allows you to drive a circle in a sketch and also to limit this value with the minimum and maximum values. I think that for this we should be able to assign the standard value to the parameter each time the configuration changes in the parameter table, but without keeping a link with the table.
If you break the link with the table you lose the possibility to configure a new diameter (unless you transfer the data to the model but the result is the same as with the table).
The Mini/Maxi terminals that can be assigned to a dimension are not accessible via the table.
What you are looking for corresponds for example to a screw hole where you would like to be able to change the nominal (via multiple choice or parameter table) and then apply the minimum maxi set?
In fact, it's for a table containing about 1 thousand O-rings. When I select an O-ring from the list, by default I create the seal with its nominal diameter thanks to the information contained in the table. Only in reality is it necessary to adjust this seal to the piston or the bore while remaining within the specifications of the use of the seal (depending on the assembly, the pressures on both sides of the seal, etc.).
As a result, I would like to be able to have control over this parameter in order to adjust it to my room. It is also possible to add a parameter in the form of an offset but I don't find it clear at the tree level and it can be confusing.
Would it be possible thanks to the knowledge advisor to apply a value to a parameter just when you change the configuration in the parameterization table?
I would like to be able to have control over this parameter in order to adjust it to my room.
Would it be possible with the knowledge advisor to apply a value to a parameter
Can you specify because point one and two are not compatible.
Adjust manually
Apply automatically
For the 1, instead of controlling the Diameter dimension by the table, I would insert a user parameter (D_cercle), then a user parameter (adjustment), finally the associated diameter sketch dimension by formula, "D_cercle+adjustment" (well, for readability, I would hide the user parameter (D_cercle).
For the 2nd of course a reaction to the change of configuration is possible
For solution 1, it's this famous "offset" that I didn't want to use because very often the "adjustment" value will not be round (for example 0.22 for a joint diameter of 1.78 to have a 2 mm dimension) and if we change the configuration there will be an offset that we will have to think about modifying... But it may be the simplest solution!
For the incompatibility of points 1 and 2, I was actually wondering if it was possible to assign a value to the parameter only when you trigger a configuration change in the table, without this parameter being associated with the parameter table.
1 Yes , with Catia you can't have several configs of the same part in an assembly, which in your case forces you to solve the catalog (create each config). So by default a joint integrated in an assembly will have this offset parameter set to 0 and can be modified. the only PB is if in the same assembly you use the same joint several times and you want different offset values between these joints.
2 You can create a reaction by selecting the "configuration" parameter as input in the graph below the table. but the parameters will be associated with the reaction so not modifiable manually unless you enter the reaction script.
That's exactly what I was looking for, I created a reaction that allows me to make an equality between a parameter from the parameter table and my parameter which, for once, remains modifiable and unrelated to the table. For the bounding I created a "message" type alert when the allowed values are exceeded.