Today we will continue our series on the hidden intelligence of CATIA V5. It is important to note that I am using a standard Classic HD2 license for this series In my last post, we discussed building a catalog of parts based on a single part that has a spreadsheet that drives the parameters with part numbers. What about features? If CATIA V5 is powerful enough to generate entire parts based on parameters, shouldn’t it also be able to be able to generate repetitive features? For instance, take a boss feature that appears on the B-Side of a plastic part. As a leader, I would not be interested in paying my designer his rates to keep repeatedly modeling a feature that may only change slightly throughout the backside! Model smarter: make once, use many times.
To do this successfully, you must address a few things – the first being how it may change. Of course you may not anticipate all changes, but a good rule of thumb is to try to model with maximum flexibility (big slabs for surfaces, overbuild everything, pay close attention to design intent) and do not use B-reps for your design. Avoid creating and building off of features CATIA builds, meaning whenever possible build your own and pick only from the tree to link to them. The second issue to address is – what are going to be the parametric numerical inputs to drive the design? See my first post in this series on how to set these up. i.e. Draft Angle, Wall thickness, Outer Diameter, etc.
Finally, what are going to be the geometric inputs to drive the design? i.e. Location point, Pull Line, Slide Line, Mating Surface, etc. A good rule of thumb here is to limit these features to as few as possible that are needed to get the job done. Sometimes it may be beneficial to sketch all this out on paper before you build it; I suggest gathering input from all the possible parties to help you in your definition.
In the example below, I have constructed a boss. Let’s review what I did.
Essentially I have two geometrical sets: a set to hold only the Inputs (appropriately named) and a set containing what I would want to duplicate (the boss feature). The number one thing to keep in mind – the theory to making all power copies work – is to keep your inputs in a separate geometric set and when all of your features have been created, your final item and all of its children will reside under one body or geo set, keeping in mind that there may be several sets contained within that final body or set. In other words, the BOSS FEATURE set shown above could have an endless number of sets inside it, ultimately we would build a power copy of that set. Also the theory is to keep in mind every single feature will somehow connect back to either one or all of those inputs.
Also take note that the INPUTS are dead (non history) based features, which is not necessarily a requirement but it does help. Essentially, when you are inserting a power copy in CATIA, it is basically duplicating a geometric set or body and all of its geometric drivers are being replaced with new drivers – nothing more. In other words, take a whole geometric set and copy it and paste it, then go into each item’s parent that needs to be repointed and do a click replace on each one – but you’re doing it all at once. The key is to design and build each feature with that in mind as part of your design intent.
Creating a power copy is easy: simply look for the Product Knowledge Template toolbar and use the Power Copy command to begin the process.
The dialog that appears gives you the option to name the Power Copy and is expecting you to pick the body or set you want to make a power copy of. Once that is selected, your inputs are automatically calculated and appear in the Inputs of the components side of the dialog. This is a good time to make sure that this list matches what you have in your defined set for inputs.
Note that if you happen to have an additional KT1 license (comes standard in PLM Express CATIA as part of CAC) that you can always check this information ahead of time by right-clicking on your set and choosing the Edit Inputs option as well.
Getting back to the dialog, at this point you can click OK and your power copy would exist in the tree. However, if you want to have your user parameters that are already set up to be included, you will need to add them as additional inputs; simply pick them individually from the tree.
Lastly, if you want the ability to change the parameters before you insert the power copy, you need to publish them. This is not the same as publishing a feature through the Tools pulldown. Simply click on the Parameters tab, scroll to locate them and select each one, and activate the Published button for each one you would like to change.
Once your power copy has been created, it will appear in the specification tree under the PowerCopy node.
Enjoy the video below of this power copy in action on a console part that needs these bosses to get an idea overall of how the process works.
As you can see, it is very efficient to already have pre-defined common features existing in a part somewhere when working on repetitive tasks. The world of CATIA V5 is all about re-use of data and capturing business intelligence we already know exists in all companies. Do you need a hand harnessing yours? Our team at Tata Technologies has helped many manufacturing companies find and leverage the unused resources they already have. Let us know how we can help!
Latest posts by Lewis Breeding (see all)
- What is the Functional Modeling Part Workbench? - August 9, 2017
- The Hidden Intelligence Of CATIA V5 – Part 4 (Power Copy) - July 5, 2017
- The Hidden Intelligence Of CATIA V5 – Part 3 (Catalogs) - June 2, 2017