This is a second look at the hidden intelligence of CATIA V5. Our topic today will focus on the creation and use of design tables. As I talked about in my last blog post, parameters and formulas can be used to drive your design from the specification tree based on your design intent. We will continue on using the rectangular tubing part and build several variations of that tubing that can be driven from a spreadsheet.
Most of the work has been already done, and although it is not necessary to have pre-defined parameters and formulas existing, the process is faster. We will begin by again looking at the Knowledge toolbar, this time focusing on the Design Table icon.
When the command is selected, a dialog appears asking for the name of the design table and also gives you a choice on whether or not you want to use a pre existing file or create one from the current parameter values. The differences being whether or not you have an existing spreadsheet filled out already with all the tabulated values of what changes in each iteration of the design.
In our case, to show the functionality we will choose the create with current parameter values option. Once that is decided, you choose which parameters you want to be driven by the spreadsheet. In our case, we had some already created, so we changed the filter to User parameters, chose the values that were NOT driven by formulas (INSIDE and OUTSIDE RADII) and moved them to the inserted side by highlighting and clicking the arrow.
At this point, we have defined that we want a spreadsheet to use columns for Height, Width, and Wall Thickness based on the current values in the model as it is at this moment. When we click OK on the dialog, it will ask us where we want to save the spreadsheet. I suggest that you do this in a place where anyone who uses the model can has at least read access to (i.e. a network drive). Note that I can also change the type of file to a .txt if I do not have access to Excel® or any other software that can edit .xls files.
Once this has been defined, your design table is created, linked to your 3D model, and ready to be edited to include your alternate sizes. This is confirmed by the next dialog. To add in the other sizes, simply click on the Edit table… button and your editor (Excel or Notepad) should launch and simply fill in rows with your values.
Once you have edited and saved the values, you can close that software and CATIA will update based on your values.
Now you would just pick the value set you want and click OK for the change to appear on the screen.
At any time, you can always go to make the changes by finding the Design Table under the Relations section of the specification tree and double-clicking on it.
As you can see, it’s pretty easy to create a design table and drive your parametric file with multiple values. The world of CATIA V5 is all about re-use of data and capturing business intelligence we already know exists in all companies. How can we help you? Tata Technologies has helped many companies time and again.
Stay tuned for Part 3!
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