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Send To Directory v. Save Management Propagate DirectoryHelpful Member!(4) 

RCDLtd (Automotive)
13 Oct 05 13:49
For an open Product in V5 (R13 & above) does anyone know of any functional difference between:

File, Send to, Directory

and

File, Save Management, Save As, Propagate Directory.

I'm trying to get a Data Management process down in writing and don't wish to be later tripped up by some subtle difference.

Thnx in advance.
Helpful Member!  Akesson (Mechanical)
14 Oct 05 10:36
Hi,

A CATIA Document is known by its file name and identifier (UUID).

By using "Send To/Directory" or "New From" you get both new file name and new UUID.

If you use the "Save As" command without checking the "Save as new document" box you’ll create a copy of your document that have a new name but the same identifier (UUID). This will cause you problem if you use both documents in the same CATProduct. The "Save as new document" box isn't avalible in the "Save Management" dialog.

Hope this help you.

/Akesson
Helpful Member!(2)  PeterGuy (Automotive)
17 Oct 05 12:44
DS documentation of this area is poor. The send to function does not give a new UUID to the files where as New from does. Save as will give the file a new UUID if the file name is diffrent from the original.
Akesson (Mechanical)
18 Oct 05 5:14
In documnetation that I have that is written by Dassault it says that "if you Save As a part, this part is renamed but keeps the same identifier".

As I see it Save as (in Catia V5) should be compared to Rename (in Microsoft programs)
PeterGuy (Automotive)
18 Oct 05 8:34
Akesson you are correct save as is not changing the UUID, which is in direct contridiction with information DS Support gave me last year (It is not beyond the bounds of possiblity that they have changed something). However the files created using save as are not identical to the original where as Send To are identical.
You can test the various senarios by making a drawing related to a part. Perform the various save operations on the part and see if the drawing view link will accept the replacement of the part with the new ones.
Akesson (Mechanical)
18 Oct 05 9:59
Hi PeterGuy,

I've noticed the problem with "Save As" when both parts with same identifer (part1 and part2) are used in the same CATProduct.  
If a Product contains part1 and I try to add part2 Catia will add another part1.

File management in Catia V5 is difficult to understand....

Maybe you have an idea how to solve the issue in thread560-128210

/Akesson
PeterGuy (Automotive)
18 Oct 05 12:50
If two parts that have the same UUID (even if they contain completely diffrent geometry) are used in a product the second file will use the master visualisation of first file put into the product. This is how V5 handles instances, the first file is loaded all files with the same UUID are considered to be instances of of that files. So you get the strange behaviour of putting a diffrent part in your product but have the visualisation of another file but performing an open in new window on the newly inserted file opens the part you expected to see in the assembly.

The general upshot is that you need to decide if the new file you are making from an existing one is:-

A revision of the original, it is going to replace the original but NOT be used along side it.

Or

A NEW Part, that possibly has similar geometry to the original but is NOT going to replace it but may be used along side it.

Dependent on the which of the senarios you are following you select the file operation command that either modify the UUID or maintain the UUID.

I aggree that V5 file & link managment is hard, it is not helped by vague documentation that does not clearly illustrate which command will modify the UUID and which will not.

I have looked again at if Save as changes the UUID and it certainly does change a UUID wether it is "THE" UUID is a good question. You can see this by create a new part & save it. Then save as the file twice using a diffrent filename each time, close the files. This file need not contain any geometry at all & the reason for save as twice is there is a big difference between an initally saved file and subsequent save as'es.

in a command window on the Windows OS run the following command

fc FileOne.CATPart FileTwo.CATPart >compareresult.txt

where fileone & filetwo are the files you have just saved
Open the compareresult.txt at around line 22 & 75 you should find some groups of numbers these are part of the UUID. This relates to line 2 if you open the CATPart file in something like textpad with wordwrap off.

However what I am struggling with is; why in the test files I have tried will the drawing view link accept the save as file.
Akesson (Mechanical)
19 Oct 05 2:18
Very interesting!

I've tried to compare the two files and Row 2 in the two parts looks identical. (V5R13sp6)

I would like to know how to set wordwrap to off.
RCDLtd (Automotive)
19 Oct 05 4:13
Well, the file compare certainly shows differences between the original and the "Save As" versions that aren't there when the "Send To" option is used. Quite what it means though is over my head.

I think my safest bet is to specify "Send To" as the command of choice for data transfer, until I understand the implications of the "Save As" differences.

Thanks for your help.
PeterGuy (Automotive)
19 Oct 05 15:27
Word wrap off in Textpad is Configure-->Word wrap

Certainly I would use "send to" if I want copies of the files with the same UUID (a revision of a part).
However, if I want files based on a starter file to be used along side the original or in somthing completly different then I would use  "New From" (a new part).

The function of both "send to" and "new from" is clear and easy to understand.

I also tend to create my revisions and new files then integrate them into my product structures rather than rely on functions that may or may not (dependent on options and whats in my session at the time)integrate the new version of the file into the structure. The main reason for this is I can evaluate the impacts of a change & make a plan to implement the changes in a no unexpected results controlled manner. The other reason is I am a Catia AE and spend my time resolving the sort of mess others make when they get it wrong.   

Save As becomes more complex still, according to DS save as does not give an new UUID if you do not change the filename. I have taken DS's word for this up to now but it looks like I am either going to have to get them to clarify the behavious (difficult) or investigate it myself (easier but takes more effort).

And as a final confusion does the "save as new file option" just mean that any file in session that references the document being saved as does not reference the new copy or does it do something more.
Helpful Member!  catiajim (Aerospace)
20 Oct 05 11:08
Another difference between Send To and Save Management/Propogate Directory is that Send To will grab any and all reference files that you may be pointing to - like your Format Drawing and any Catalog Parts (including the Drafting Catalog source!).  

We have not had any problems with Save Management/Propogate Directory changing the UUIDs, although I have never compared them via notepad.  I just know that the behavior is OK.

A better option that we have found is under the DMU Navigator workbench (if you have it).  Under the Tools pulldown, go to DMU Data Management, and select SAVE AS FROZEN.  There are a number of options here that are very useful.
RCDLtd (Automotive)
21 Oct 05 4:17
Hi catiajim, from you first statement are you saying that "Save As/propagate" will not necessarily collect the associated "Format Drawing and Catalog Parts" into the defined directory.

This is really the crux of my question. ie. How to robustly send data out to a third party so that it can be worked on and returned back with all associations and links still in tact. And of course, when it does return to still be associated to the original data and not content that it now considers to be unique.
catiajim (Aerospace)
24 Oct 05 8:37
Yes, it does not pull them.

As for your second question, it is really 2 problems.  If you send out your drawing & product via  "Save As/Propagate" you won't get the reference documents.  However, your supplier will still be able to work on the drawing and parts.  When they send the data back to you, the links, which should still exist, will be resolved again - that is assuming that your supplier didn't make any new links, like to their drafting catalog.

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