Hello, little challenge:
What is the simplest and most effective method to copy an assembly with all the parts without there being any connection to the assembly and the original parts?
Hi Alain,
The most effective is the Composition to go.
When we use EPDM, we go through the tree copy.
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you have to register your assembly with another name and break the links
but for the parts you will always have a link since you don't change the name of the parts
or you also have to change the names of the parts and replace them
@+
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Hello
A small challenge then met.
Indeed, the composition to take away is the function to be used.
By paying attention to the different options offered, of course.
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Thank you @Benoit, a good answer but I don't have the EPDM.
The Take-Away Composition, ok but what setting? By default, we have every chance to keep the associative side of the parts files.
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Hello
If all documents are checked and include drawings is checked, there is no longer any link to the original files. But of course you have to choose another file!
And you can add a prefix so as not to confuse it with the original project (we use AVP_ for pre-project).
More info:
http://www.mycadblog.fr/composition-a-emporter/
Edit:
But we use the save as macro that I created (available on Lynkoa), because during the study, we don't yet know if we are going to reuse existing parts, so we first save the highest level assembly, then the parts we need, one by one. This avoids duplicates and avoids overloading the server.
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What links do you have in mind? Do you have any parts edited in the context of assembly?
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FYI, in the "Composition to go" dialog box you can directly change the name of future files.
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Via the ProjetcManager utility (it's like the "take-away composition" of SolidWorks but more complex).
Of course, you have to add a PREFIX or a SUFFIX to all your copied project (parts, assemblies and plans).
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This is a generic molding tool that I want to quickly duplicate multiple times in different folders of course. There must be no link between the different projects, otherwise, it's a disaster.
I forgot to mention that the part names must remain the same, but not the assembly name.
A quick way I found is to use the SolidWorks Explorer and do a Copy and Paste but in a different folder level than the first one (otherwise, strangely, the link persists)
I couldn't do it with Compose to Go (without changing the name) or with Save copy as and continued (and the advanced options ... Save all as copy)
Are you pointing to a new file?
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"I forgot to specify that the names of the parts must remain the same, but not the name of the assembly"
That's not a good idea.... you have to add a PREFIX or a SUFFIX.
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In fact, copying and pasting as you do is the same as a take-away composition.
All you need is for the folder in which you store it to have a different name (the top level). He will then be able to remake his own links.
On the other hand, the advantage with the take-home comp is that you are sure not to forget any file and that you can rename ... The disadvantage is that from time to time he doesn't want to do it by arguing that the name is too long (since he takes into account the path in it).
I don't know if my colleagues have indicated it, but don't forget to uncheck "single file (flat)" ... otherwise you have everything under the same folder
sans_titre.png
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Hello
I agree with Flegendre; you have to add a PREFIX or a SUFFIX. It could create conflicts when you ram this assembly into another with parts that have the same name but are different.
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I think I have at least one clue to my problem: I don't close the old assemblies and when I open my "copy" it recovers the parts of what is already open and not necessarily the right part.
I had forgotten that SolidWorks prioritizes RAM above all else when searching for references.
I keep checking if I don't have any other raincoats in my references.
@Flegendre, it would be easier if I had changed the name, (see just above) but I was asked to have copies with the identical parts (inf sole, ...) in each copied folder. And it's true that it's harder to obtain...
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simply add a number after the name
The name will be the same for your assembly and your parts
but if you don't make any changes to the parts no need to change the name
A part can be in multiple assemblies
This is only necessary if you modify the parts which in this case will not be identical to the mother part
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SolidWorks (sometimes, for no real reason) is able to go and get you a duplicate part in another directory, and therefore create conflicts (crashes, etc....) that's why this solution is for me to be BANNED.
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If you have already made your assembly copy, you just have to repoint the right parts before opening... (or at least the right repertoire) good luck if you have lots of pieces!!
But rename your pieces anyway, otherwise good luck for the future!
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The only other possibility you have is to keep the same one for the part but to make configu with a reminder of the name of the folder to which it belongs.