Changing Drawing References

[SWISGR8]

I am trying to change the referenced assy in a drawing with a very, very, very similar one by doing the old "open", "references", "dbl click", select new file, and it shows the change in the New Pathname column, but when I open the file, the old assy is still there in every way.

What am I doing wrong? Isn't this supposed to work this way? Is there a setting(s) I need to ensure is(are) correct?

Thanks,
"Frustrated"

 

[handleman]

Try temporarily renaming the old assembly file so SW definitely can't find it.

 

[SWISGR8]

That allows me to change using the "...cant find ... want to find yourself ..." deal, but I thought the whole pt of the "References" in open or save was to be able to redirect the referenced location and or file name without having to go through all that?

Thanks for the reply,
Mike

 

[mncad]

Make sure that you are opening the file as soon as you are done changing the reference (while the drawing file name is still highlighted). If you don't open the file immediately it will still reference the old file.

mncad

 

[SWISGR8]

I do I think. After changing the ref, I select "ok" to get back to the open dialog box and then I open the dwg but it is still the old ref.

Are you saying it should in fact be changed at that time (that's what I thought).

Thanks,
Mike

 

[rgrayclamps]

Hi, SWISGR8:

Did you save the new created assembly drawing document? If you did not, you won't see the new assembly model referenced in your new drawing.

Good Luck!

Alex

 

[SWISGR8]

Yeah, did that but still old ref.

Let me just give the whole thing to all you in case I am doing something really wrong:

I have 4 dwgs that will be very similar in that the assy files they ref are all very similar. So I made the first and saved it 3 different times for the rest of the p/n's. My plan was then to change the refs as I opened them. And that's where I ran into my problem of refs not changing for me.

Does that all sound legal within SW?

Thanks,
Mike

 

[handleman]

Are you checking the check box in front of the new path? If you don't check the check box it doesn't actually change the reference.

 

[SWISGR8]

Yeah, checked box, but it seems to me like that is only to indicate which refs you want to do text operations on for paths, etc. But either way, I have had that checked as well and i've tried the saving. Does what I described for what I was trying to do make sense and seem like it should work?

Thanks,
Mike

 

[pdybeck]

What version and sevice pack are you on? We had this same problem at 2006 SP 2.0 and 3.0. I can say for sure the bug is corrected on 2007 SP 0.0 and 1.0. It must have been corrected somewhere in between 2006 3.0 and 2007 0.0 with a service pack or major version. We handled changing references by using SolidWorks explorer to copy the drawing and assembly at the same time and re-name while doing so. The other way we handled it was to place the file that you are switching from referencing into a different folder, so that it can't be found (this has sort of been mentioned already). Then you should be able to manually browse and select the new file, without the reference reverting back to the old one.

Pete

 

[SWISGR8]

Prof 2006, sp4.1

That must be it. I've done ways you and handleman mention, but in this case, re-directing at OPEN seemed quicker and more convenient.

What you say must be it though, because it doesnt seem like such an involved process that would make it so tricky.

There is at least one more sp but we havent had a chance to update yet.

Thanks everyone,
Mike

 

[rgrayclamps]

Hi, SWISGR8:

I have a feeling that you did not replace the model properly. Can you list all the steps you use to open a drawing (drawing "A") with refernece to a model (model "A") and redirect the drawing to reference to a different model (model "B")?

Alex

 

[SWISGR8]

Ill list step-by-step:

1)Open file

2)Select, from the file list, the .SLDDRW file which refereneces assy model "A" (with intention of changing ref to assy model "B") but do not execute opening

3)Select the References... button in OPEN dialog box

4) Dbl click, from the References list, the file (which in this case there is only 1) for which I want to apply the re-direct which initiates the an OPEN dialog box

5) Select and accept the file (assy model "B") from the list

6) The "New pathname" column now reflects this change

7) From this point I have tried all combinations of:
- making sure the box of the reference I changed is
checked before executing opening
- open in lightweight on/off
- save after opening to see if that effects change
- Rebuilding/Forced regeneration/Saving-closing-opening

Let me know if something seems incorrect.

Thanks,
Mike

 

[pdybeck]

Mike,

Your process is correct. Alex assumed that you did not apply the change correctly. It is a bug as I stated earlier.

Pete

 

[SWISGR8]

I'm figuring that it is a bug too, and as long as all agree with process makes me more confident.

Thanks everyone,

Off to get SP 5.0

Mike

 

[nathonrose]

So, you have 4 models:
Model A, B, C and D
You made a first DWG A which References (->) Model A.

To be clear, you need to:
Open: DWG A -> Model A
Save As COPY: DWG B which will still reference (->) Model A

Save As COPY: DWG C -> Model A
Save As COPY: DWG D -> Model A

Then close DWG A.
Open DWG B, then go into the references box and change the reference to Model B, as you listed in steps 3 and on.

This should work, I had it work in SP4.1, I believe. As that is what we had until just recently when we went to 2007SP0.0.

It sounded from your list that you may have just opened up your orignal DWG A and wanted to reference B and THEN do a save as. That won't work, for some odd reason.

 

[SWISGR8]

What you say is what I did. I even just did it quickly to make sure I use the saved-as-copy dwg and still no go. I also got up to SP 5.0 this noon and still no go. Looks like SP 5.0 is latest, so I am going on hope that once we get to 2007 all will be fine. It's not a huge deal I guess, I mean there are work-arounds, it just seems very convenient in this case.

 

[rgrayclamps]

Hi, SWISGR8:

I do not think there is a bug here. Your steps 1 to 6 are fine. But the step 7 may have problems. You did not indicate whether you save your active drawing document as (or as a copy) another drawing document.

I have been using SW 2006 sp 4.1. I do not have any problems at all. You may want study a lot more about SW search mechanism ("Searching for Referenced Documents") using SolidWorks Help Topics menu. This section talks about search priorities in SolidWorks.

Also, take a look at Tools/Option.../System Option/File Locations/ to see what you have for referenced documents.

Good Luck!

Alex

 

[nathonrose]

I don't know if you can post files here, or attach an HTML link, but, you could do the SolidWorksRX thing to record your steps to a video file, post that and then maybe we could comment. I'd say it could be a bug on your install, but since you upgraded that should be cleared.

It's a settings issue as RGRAYCLAMPS states, or "pilot error" we just can't see what's happening.

I'll try to do a video myself for you and post it if I can.

 

[nathonrose]

Blurry First Try:

http://video.google.com/videoplay?docid=5334921636590221410

Will try again. You can note that the preview when I go to open up any of the drawings the first time, shows the preview image containing Model_A. But when I open they are the properly newly-referenced models.

I'll try for a cleaner video.