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How to interconnect the published geometry?

MrCATIA

Super Moderator
Monstrobolaxa asked the following question in a private message:

Hi MrCATIA
I-d like to thank you for the help you've given me on a few ocasions.
Quick question about "publication"! I understand how to do it on single parts...the question is how to interconnect the published bits with a new part that is being made?
For instance if I want published axis to be used on a new part I'm drawing?
I've never used CATIA in a very professional way...mostly academic stuff or very simple assemblies, but now I'm looking at further developing my skills.
 
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MrCATIA

Super Moderator
One way to use Published geometry is with Contextual Design

1. Create an assembly containing several parts including the part with your Published axis. This assembly is the "context" for how these parts interact with each other.

2. Let's call the part with with Published Axis PART1, and let's call another part PART2

3. Expand the assembly tree so you see the Publications in PART1, and expand the tree to also see the PartBody in PART2. We will be using the tree to make most of our selections.

4. Double-click the second line of the tree in PART1 to make PART1 the active part where we want to work. This will show a blue background in PART1. This will also switch workbenches to the Part Design workbench

5. Add a new Plane in PART1. And publish the Plane, just like you published the axis.

6. Now double-click the second line of PART2, so that becomes the active part (blue background)

5. Now let's make a new Sketch for a Pad we will add to PART2: For the sketch support, select the Published Plane in PART1. Add a profile to the Sketch, and use this sketch to make a Pad

6. That's it! You just select published geometry in other parts to use within the part you are working in.

7. If you look at the tree of PART2, you will notice a new branch has been addded called EXTERNAL REFERENCES. And inside this branch you will see a Plane that has been copied from PART1 with a link back to PART1. There will be a blue/green "P" on plane symbol, indicating that it is published.

And if you look at the icon in front of PART2 you will see two little gears colored blue and green. The green gear indicates that PART2 is "contextual" in that in contains contextul links that have been "imported" from another part.

8. If you go back to PART1 and modify that Plane, then the linked plane in PART2 will change also, modifying the sketch support and the Pad that were created from it.

9. Working like this in "Contextual Design" mode is good because you can design all the parts around all the other parts.
 
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MrCATIA

Super Moderator
I forgot to mention in Step #5 above, you will probably get a pop-up message when you select the plane in the other part.

The message depends on how you have your Tools+Options set, but the message is confirming that you are "interconnecting" geometry from another part into your current, active part. The Part Infrastructure page has the options for working with links.

Also, I described the blue and green icon indicating a contextual instance of the part in the assemblyl. Most part instances will have a blue and yellow gear icon, which means the part is not contextual and has no Imported links.
 

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