Fully constrained parts

[huntwe]

Is there a way to tell if a .catpart is fully constrained in a product by looking at the tree? In solidworks you could tell at a glance, the undefined parts had a minus symblol in front of them.

 

[itsmyjob]

With CATIA by default , NO.

But if you have rules in your CATPart, they can check if sketches are fully constrained and also if you have datum element. As the result of the rules are in the tree as a green or red light, you might be able to have the information your need by looking at the tree.

Eric N.
indocti discant et ament meminisse periti ​

 

[ferdo]

Hi,

In assembly workbench, right click on component, name of the component.object - Component Degrees of Freedom

Regards
Fernando

 

[tuzoenduro]

This also works if you go to Analysis (in french is analyse so I don't know in english) you have Constraints and Degrees of liberty...
there you can look over your complete product...

 

[mymylepire]

Hi,
It is actually analze.
Forst, double-click on the part or product you want to make it blue. Then, Go in analyze (menu at the top next to tool) and selcect Degrees of freedom.

Myriam

 

[huntwe]

My intent was to find a way to quickly scan over the tree and tell at a glance what parts were fully constrained and what parts are not. In a product with 50 or more parts it is not really effecient to find the degrees of freedom on every part. If I replace a part or take a part out and it makes another part un-constrained I will never know it. If that part gets moved in any way them my product is not accurate, and I will not know it. This is a problem.

 

[Solidkat]

When your parts are in the rigth place why not just use the fix command.

 

[jackk]

Solidkat: that's an easy way to do it, but what happens when a part changes? or a mounting hole is repositioned?

Huntwe: a quick way to check constraints is to explode the assembly and then update - the parts that don't go back to the correct position are not constrained.

 

[Solidkat]

Jackk: if the parts are going to change then it comes down to modeling practices and design intent.

 

[jackk]

Solidkat: if your parts are designed in airplane coordinates, then Fix makes sense. But lots of parts aren't. I believe CATIA was written based on the modeling practice of constraining parts within assemblies. Try the explode&update test with your fixed part assemblies. What happens to your fixed parts after you accidentally move them with the compass?

 

[Solidkat]

Jackk: all our parts and sub assemblies are on local coordinates and only the top level assembly is on aircraft coordinates. It’s company policy not to use constraints so all parts are positioned using snap and fix. The job is made easier by publishing geometry at the part and assembly level. If any of the parts or sub assemblies is displaced by the accidental use of explode or errant compass use, a quick click of the update icon returns all parts back to the original location.

 

[jackk]

Solidkat:

Thanks for the explanation of your company procedures. If the parts stay where they belong, then it's good. And I stand corrected.

I was taught to use assembly constraints, and most parts I work with are not modeled based on a master axis system (airplane coordinates). I will try the Snap & Fix method.

Thanks for your persistance in making me aware of another method, and proving again that CATIA provides the flexibility to accomplish things with numerous methods.

Jack