Internal IDof Document does not match

Hi folks,
I'm getting the following error when trying to open a large assembly
file.

The internal ID of document D:\Work in Progress\MARS\Shower Trim Cell
\High Level Conveyor.SLDPRT does not match the internal ID saved with
the referencing document. Select YES to accept this document anyway.
Select NO to browse for a replacement model.

It's only become a problem since I saved everything out as a STEP file
so that my client could read it into their system. I opened up the
STEP file to check it was okay and I suspect that this is where the
confusion has arisen.
If I get rid of the STEP files will SW then pick up the right parts
again or will I have to manually point it in the right direction? Not
a task I want to do if it can be avoided.
I can open the sub-assemblies okay, it's just at the top level
assembly where it cause me a problem.
Thanks,
David

 

David,

It's often helpful to check the results of files exported in non-
native formats by translating them back into SolidWorks. This way, if
the recipient of your exported file complains about not being able to
read it, you can usually rule out corruption.

To avoid the 'internal ID' problem in future, I'd suggest that you
simply avoid having the imported results of your STEP file open in
SolidWorks before you open the navtive assembly from which the data
was exported.

By default, while opening an assembly, SolidWorks will prompt you to
'adopt' an already opened file if it has the same name as the part
referenced (in the assembly) when it was last saved.

It's a good idea to export your STEP and other such files to a
directory other than where your native SolidWorks files reside.
Importing the data files from a separate directory will also help with
file management.

Per O. Hoel
_____________________________________________________

 

Opening the STEP file created files of all of the assembly components
with the same name as the original. These will not have the same
internal ID.

Find the re-translated files and delete them. Hopefully you haven't
overwritten your originals.

To reconnect your assembly with the original component, simply open
the component before opening the assembly (and then save!).

 

Thanks for the tip That70sTick. I'll try it tomorrow. Fingers crossed.

 

It's time to dust off some options.

In the system options there is a check box for search external
references.
In the file location area there is a Referenced documents file path(s)
you can set.

By checking the former and setting the later you can tell SW to look
first for files in location where you expect them to be.

The root of your problem is that you have two different files with the
same name and SW got a hold of the STEP related file and thought that
was the file to load, hence the file ID warning.

You have to be very careful in SW to make sure you have unique file
names for all your files or you will run into this and many other
problems. SW has a very thorough search routine and it will sometimes
find a file in the strangest places if it exists and throw off your
assembly or drawing. In other words if you recreated your files from
STEP you should have changed the names in some way like adding a -1 or
something.

To compound this problem a file can existing in memory silently. You
won't have any way to know it is loaded, but if it has the same name
as a file in a folder and you think you are loading that file, you
aren't because SW thinks it is already loaded. Although SW stores the
file's nam and path, when in memory it only uses it's name to
determine identity.

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