Catia Users

Hey,

For any project with more than 100+ parts I usually create sub-assemblies and a Final Master assembly. I create folders according to the sub-assemblies. Remember, you cannot change file location after creating an assembly file.

To create folders for parts in catia itself, I haven't seen any option, there might be one since catia is very vast. In industries, assemblies with 500+ parts I have seen professionals create classes of sub-assemblies in catia. I have been doing the same since then. But there are different ways, I wish I could help you more.

Hello,

Thanks for the quick reply... If I understood you correctly, you open a blank product, insert parts needed, constraint them and then at the end of your work you create products inside the main product and then drag and drop the parts in them(therefor creating sub-assemblies), no?

If that is your method I would like to know if your constraints gain a yellow "!". More on if the yellow "!" even matters... If not please further explain, so to say I am quite lost :)...

All in all, if Catia has that kind of feature, they should invest in making it more known... Anyway, thank you.

Teo C.

Did you happen to capture the strange "action not possible" message? It probably had a clue about what was causing the problem.

Try double-clicking on one the broken constraints (with the yellow ! symbol), and see if there something there about what is causing the assembly constraint problem.

Use Edit+Links or File+Desk to make sure all the parts are loaded into the assembly (I suspect this might be the problem)

Do you normally use the "work with cache" option? Could you have switched into Visualization mode by mistake?

Hi Jack,

The message unfortunately I did not catch.

I have clicked on the broken constraints and they had the tabs "Type" and "Component" saying "Unknown" and the status tab "Disconnected".

I am positively sure that all parts were loaded in the assembly, therefore I do not think that is the problem.

I do not use "work with cache" at all.

Furthermore I think I still do not understand the process that was mentioned by Anirudh Rao, and therefore making the mistake in that step. Once again I will repeat my process and please correct me if you see the mistake/s. I started a blank assembly, imported parts and constraining them as they needed to be, now at the end I am inserting components, renaming them to suit the needs and one by one dragging and dropping parts in them. After an hour or so of sorting I have found that all my constraints were broken and said the thing mentioned up above. After that I opened a backup and kept working in it.

Thanks for any effort spent on this thread and all the advises in advance.

Teo C.

What do you mean "renaming them to suit the needs?"

Are you renaming the CATIA files?  Or, are you just renaming the part instances within the assembly?

I am renaming the newly created components in wich I would drag and drop the parts.

Example of this may be, I have assembled my product and have many bolts M10x90, I inserted a new component and rename it M10x90. Then I procede drag and drop the parts in that component.

Is this the error I am doing? Because I still do not understand :).

Teo C.

That's OK if you are just renaming the sub-assembly component.  We are talking about components that have this symbol in front of them - right?

It is not OK if you are using FILE + SAVE to rename anything in the assembly

Yes yes we are talking about the same simbol, I rename them and keep untuched the names of the parts. Only thing I do is move them from the main assembly to the component, therefore they somehow loose their constraint properties and break the constraints.

I am realy confused, for all I wanted is to tidy up the assembly for better managing and that taks I can not do. I do not know is it the lack of knowledge or understanding for the program...

Thanks for all the help and time spent, if someone is successful at this task please do share your methode.

Teo C.

I understand you constrain the parts and then drag and drop the parts into new components. Maybe you can add geometrical constraints later, after inserting all parts into respective components using transform tool or snap tool. Once all your parts & components are assembled according to your requirement, you can constrain them then.

I would suggest you try this with a smaller assembly first to avoid wasting time with the original one.

Sorry I think I did not understand you. You are suggesting I should constrain the whole assembly, organize it and than constrain it again? I think that is not the good way hahahaha...

If anyone knows a way please do share your method. All advises are helpful and thanks in advance.

Teo C.

Teo,

Try this:  right-click on the component, and then click the FLEXIBLE/RIGID option.  (Flexible sub-assemblies will have a pink symbol)

Hi Jack,

Yes I have tried this too, before and now, just have checked again... This does not work too... :)

Teo C.

I had the same problem as Teo. After inserting all the nuts and bolts into an assembly if you want to re-organize them the correct way is exactly what he did. He created a new "Component" which does not have any external file links and he dropped all his bolts into the component.

Nice way to clean up the tree!!

However when you do this you will break the constraints. To solve this go to Tools<Options<Mechanical Design<Assembly Design then go to the "Constraints" tab and in the "Paste Components" make sure the "Always with the assembly constraints" radio button is activated.

Now when you drag and drop your parts around the tree you will not break the constraints.