The Hidden Intelligence Of CATIA V5 – Part 3 (Catalogs)
This is Part 3 in my series on the hidden intelligence of CATIA V5. To quickly recap what we have already talked about, in my first post I discussed the importance of setting up and using parameters and formulas to capture your design intent and quickly modify things that you know are likely to change. We took those principles a bit farther in my second post and discussed the value of building a design table in those situations when you may have a design with parameters that will vary and that you want to use many times. In that case you could see that we had our rectangular tubing part and could modify its wall thickness, height, and width to make several iterations of basically any size of tubing one would ever need! You would simply keeping doing a Save as… and placing those parts in your working directory to be added into an assembly at some time (I assume).
This methodology would work fine, but today I want to focus on a very cool spin on this theory by building a catalog of your most commonly used parts which are similar enough to be captured in a single model. Using our tubing model, and picking up where we left off, we have a spreadsheet that defines the parameters that change. All we would need to do to build a catalog of each iteration of the design table is add a column to the spreadsheet named PartNumber just as I have it with no spaces in the name and then associate that to the ‘Part Number’ intrinsic parameter that is created automatically when you being a model.
Let’s get started. I will open both the model and the spreadsheet, edit the spreadsheet with the column, and then add in some part numbers.
When you save the file, the field should appear in CATIA when you click on the Associations tab.
Scroll in the Parameters field to find the Part number parameter to associate to the Column.
Simply click on the Associate button to link them up.
Click OK once you have confirmed they are associated to each other.
As you can see, the Part Number from the spreadsheet is now driving the field in CATIA. We have completed the minimum requirements needed to build a catalog of all the iterations. We would now switch to the Catalog Editor Workbench.
You will then automatically be in the creation stage for a new catalog. Here you could either open an existing catalog or you can edit the name of the chapter of your new catalog; we will call ours Tubing.
We would now create a part family based on our model that contains the spreadsheet with the PartNumber field associated to the Part Number parameter. This is a requirement for this method to work. On the Chapter toolbar, find the Part Family icon.
In the dialog, create a name for your family of parts and select the document that meets the criteria; click OK in the dialog.
Finally, expand the tree, right-click on the new family, and Resolve the files. This is where the magic happens and the parts are created.
As you can see, if I double-click on the tubing family, a list of parts appears.
If I click on the Preview tab, you can also see an image gets created for each new part.
Now all that’s left is to insert these pieces into an assembly and adjust their lengths, and you’re off to building structures. Enjoy the video below showing this portion in action.
As you can see, it is very efficient to have pre-defined common parts in a catalog when working in assembly mode. The world of CATIA V5 is all about re-use of data and capturing business intelligence that we already know exists in all companies. How can we help you? Our team at Tata Technologies has worked on projects like this with many companies time and again – don’t hesitate to let us know if we can be of service.
Stay tuned for Part 4!