Reoccuring Error message "already-open document"

So I opened four drawings from the open window in SW16 at the same time.

Three reference different models, while the last is an assembly and references two of the models from the other drawings.

I received a message:"The document being opened references a file with same name as an already-open document." which had an auto-dismiss.

It chose to "Open without this document" and I just went with it to see what would be suppressed and thus not referenced.

There were no missing references... so I just ignored it.

Five minutes later the same message has popped up twice... yet I have not opened any new documents.

It just keeps popping up even though I already dismissed the message in each drawing.

In the time it took to type this post I had to dismiss six more messages!

What is SW doing???

SolidworksDrawings And Detailing
Answers 7
SC
SC 2016-05-23 Best Answer

Check the file references for each of the 4 assemblies.  I'd bet you have that file in more than location.

Steve C

RW
RW 2016-05-23

It means you already have duplicate parts, and that the one you have open isn't the one the assembly has referenced.

This is a fairly benign example of the ills duplicate parts can cause. You can end up with changes to your design that aren't apparent because the assembly is referencing the incorrect file.

Best practice is to rename files when copying, or just reference the original.

AW
AW 2016-05-23

SolidWorks is doing exactly what you asked it to do.  Not necessarily what you think it is doing.

I agree with Steve and Robert....

Check under File > Find References after you open your assembly.  I suspect you will find that the files are not opening from where you expect them to be opening from.

Each file should have unique names.

Also a good practice to close SolidWorks completely when your are opening assemblies after copies and clones to be sure to flush memory.  Lest you end up with surprises on where your part/sub-asm files are located.  Especially important if you have files with the same name in multiple locations.

SD
SD 2016-05-24

I only have 1 assembly, but references checked and all files are in one location. no duplicates.

SD
SD 2016-05-24

No duplicate parts, and the assembly references correct part files in correct location.

SD
SD 2016-05-24

Thanks Anna, I didn't know about the File>Find References function!

I used to check the references with the Reference button before opening a file.

Using the Find Reference function nothing looked wrong

...but upon further inspection and checking "Include broken references" I got a surprise!

Somehow I have a part which references an assembly that doesn't exist???

I will have to investigate further.

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SD
SD 2016-05-24

So I was able to find the external reference I had in a sketch and delete it.

It went back to a desktop version of the file from I-don't-know-when!!

Weirdly the broken reference didn't affect the file in any other way... no warnings or caution symbols... if that message hadn't popped up a million times I wouldn't have even known it was there!

Thanks a bunch!

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