copying designs withou vault...how?

[jschaap]

dear all,

i do not have vault installed since i am a single user and after installing it it made me "crazy" setting things up and wondering where the files actually are (file structure) concerning backup..

so my question is as follow. when i copy a map with all its parts (assembly, dwg, parts etc..) to a new folder in windows explorer, i have the option to replace the parts in the assembly with the ones in the new folder. unfortenetly inventor uses absolute paths for references and not relative paths, which would make things easier. so when i have done this and the assembly is again all completed with the new parts (what a drag!!) i bump into the following problem...

the drawing (.dwg) does not update and keeps absolute reference to the old folder (assembly, parts..) and there seems no way?? to update/substitue this to the parts of the new folder, since when i double click on a (base) view, i cannot use the browse button to select another .iam... it is greyed out. is there a way to do this? it would be a drag i guess also, but at least i do not have to setup my drawing all over again...

now the conclusion of all this, does anyone know a good way to copy a design to a new folder and 2make it work" without using vault??

thanks,
john

[Anonymous]

what version of Inventor? if 2010 do you have the subscription advantage pack tools?
have you searched this forum for this topic (its been covered a 1000 times)
have you considered buying a book on Inventor? I just flipped througfh the one on my desk and this is covered in there.

click this link for one method on how to copy an assembly
http://docs.autodesk.com/INVPRO/2010/ENU/Autodesk%20Inventor%202010%20Help/index.html?url=WS1a9193826455f5ff5f7e8f111d48518713032.htm,topicNumber=d0e191396

once the link is open click the procedure tab and for step 9 use "Open in New Window". This creates a new assembly file copied from the original.

As far as linking the drawings you can do this with 2010 subscription advantage pack tools
other wise you have to trick the IDW

Search for Design Assistant for another method, where you copy the model and IDW at the same time.

Note that if you are working with Frame Generator assemblies DA will not work, so there is yet aother method/tool you would need to use.

[Anonymous]

The solution is to learn about Project Files.

http://teknigroup.com/AU2007
--
Dennis Jeffrey, Autodesk Inventor Certified Expert

Subscribe to the free "The Creative Inventor Magazine now available at:
http://teknigroup.com/CI-Subscribe-Login.asp

[jschaap]

thanks for the advise. i am using design assistant and it does do the job for me

john

[Anonymous]

Hello

i have tryed the copy in another window and it works it brings the whole assebley over but i does not bring the part numbers over. it uses the description as the part number is there a way to fix this?

[IgorMir]

First - use Pack & Go. Don't forget to collect the drawings too. How to - was explained on this forum many a times.

Secondly - start Inventor and set you Project File to the one created by the Pack & Go function.

Then open Design Assistance and do re-naming of files in there.

When you are finished with the editing - close the Design Assistance and start open drawing files one by one. You will have to resolve the link for each of them by pointing into a new, re-named file.

After that you can move all the files into your working directory.

Best Regards,

Igor.

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@Anonymous wrote:

now the conclusion of all this, does anyone know a good way to copy a design to a new folder and 2make it work" without using vault??

thanks,
john

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[SBix26]

If you first use the lower pane to find linked files (drawings, presentations, derive part base files, etc.) and change the Action to Update, these links will be updated by DA when renaming the files in the upper pane.  No need for manual open and resolve link.  However, the filenames of the drawings will have to be changed individually outside DA, if needed.

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@IgorMir wrote:

...

When you are finished with the editing - close the Design Assistance and start open drawing files one by one. You will have to resolve the link for each of them by pointing into a new, re-named file.

...

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[IgorMir]

Yes, that's right, thanks Sam.

Needless to say that I didn't use that option myself. That's strange limitation with the renaming the file itself. Why not for drawings? Assembly and part files names can be edited... I will give it a shot anyway.

[SBix26]

I don't think that the limitation is on the type of file, but that top-level files can't be renamed in DA.  If you open DA from a subassembly, that subassembly can't be renamed in DA.  In trying to figure out why that limitation exists, I guess that the subassembly example might explain it-- if you rename that subassembly in DA, it could be breaking links in higher-level assemblies that you aren't aware of.  Purely speculation on my part, though.

DA is a useful tool, but it really needs a makeover to make it even more useful, more intuitive, and less annoying!

[stevec781]

In the installed folder is a directory called SDK.  Follow what the readme file says to install the user tools.  Once installed you will find a directory called Copy Design which has a tool for copying designs and has the source code.  You can edit the source with a free download of Vb.net and get it to rename etc as you want, or you can just use it as is.

I use it to copy all files to a new project directory, change the file name prefix and update all the links.  It works great.

[IgorMir]

You can say that again!

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@sbixler wrote:

DA is a useful tool, but it really needs a makeover to make it even more useful, more intuitive, and less annoying!

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[Anonymous]

How do you trick the IDW???

[SBix26]

Starting with A.iam & A.idw, copy both to B.iam & B.idw.  Rename A.iam to xA.iam (temporarily), open B.idw.  It cannot find A.iam, so it asks you to find it, you choose B.iam, save & close B.idw.  Rename xA.iam back to A.iam.