Linking problem 1

[yusf]

hi all,
I will try to explain my problem step by step to make better explanation..
Well

1.)I created a master geometry(MG) which includes some planes

2) and took some geometric entities (planes)from MG into another CATPART (CP).via Edit/Paste Special menu..


3.)and in CP i created a profile in one of plane then a part using Rib command...

4) Then after closing and saving all doc's ,from File/New From i opened CP and replaced this plane, onwhich there is my profile, with another plane taken from Master Geometry(MG) and i saw that my part is created simultaneously on the new plane...everything was ok up to this point and saved that with another name let say LASTPART(LP)

Now My question is that i want the LP to be changed after making some profile modifications in CP..in another words i want it to be u?dated when made some changes on CP...but i couldn't succes this...i think i am having some linking problem can any one help me in this point...

thanks in advance

 

[jackk]

Yusf.... I think your problem is the way you're saving your parts. Whenever your working with multiple models and creating links between them, ALWAYS use FILE+SAVE MANAGEMENT to save and rename (SAVEAS) the parts. SAVE MANAGEMENT makes sure your links are good.

I guess we could go back and fix your links by replacing them... but I think your best solution is to take your MG part and use it to make brand new CP and LP parts and save everything with SAVE MANAGEMENT.

 

[catiajim]

When you are creating a second part from the first one, always use FILE/NEW FROM, not just SAVE AS. NEW FROM will re-set the UUIDs in the parts, and will let CATIA know that they are really 2 different parts, not just 2 versions of the same part.

Also, in order to keep the two parts synchronized, you need to link them. Currently, you have two versions of the same part (regardless of File Name or Part Number) that are both linked to the Master Geometry Part. There are no links between CP and LP. There are other ways to get this, but I strongly suggest you stick with putting ALL shared geometry into the Master Geometry part(s).

 

[yusf]

"There are no links between CP and LP. There are other ways to get this, but I strongly suggest you stick with putting ALL shared geometry into the Master Geometry part(s). "....

Catiajim could you please explain your above comments in details..i followed what you both wrote and now i see that there is still no link btw CP and LP. As you stated above..how can i link them and see the updated LP when i make some changes on profile in CP..just same as product part when we make modifications we can see the changes simultaneosuly in the product part....

thanks in advance...

 

[catiajim]

You need to use what is commonly known as the Skeleton Method. In your Product, you will have one or more "Skeleton Parts" that contain all of the control geometry - surfaces, planes, sketches, points, parameters, etc. Any of this geometry that needs to be shared with other parts should be Published. Each of your child parts will then reference back to these Skeleton Parts for their shared geometry.

You can use the COPY/PASTE SPECIAL/AS RESULT WITH LINK, or you can use Contextual Links (TOOLS, OPTIONS, INFRASTRUCTURE, PART INFRASTRUCTURE, KEEP LINK WITH SELECTED OBJECT) where you are working in a product and you simply select the geometry from the other part. I strongly suggest you also turn on the LINK ONLY TO PUBLISHED ELEMENTS option on the above panel as well.

Usually this method only has one "Skeleton Part" that contains all of the shared geometry, but it can actually be several parts. We currently separate our Loft Part from our Control Part - Loft contains only the exterior surfaces and curves of the aircraft, and the Control Part contains all of the interior control geomtry like spar planes and rib planes.

There is more information on Links available from

http://www.catiacommunity.com.

You can also search the online forums for keywords: Skeleton, Links, and Context.