MODEL DETACHED FROM DWG.

[monge]

Anybody that my have the same problems out there?, when I open my dwg. my model is detached from the dwg. that means that if I made changed on my model they do not update on my dwg. when I open it, and you can tell right away when you see a blue dashed border on your views, and a message appear
that said " the following sheets contains views that are out of date with the external model"
Any help on the suject will be very much appreciated

 

[Demojock]

Hi,

it could be one of possible 2 things but first things first, does your drawing update when you rebuild it? (click on the traffic light icon typically in the upper left area of your screen) If it regens correctly then no problem, you have the "automatic rebuild of drawings" option ticked off in your settings, either manually rebuild as decribed above or go to your drawing options and tick the "Open existing drawings with automatic view update off" option.

It is also possible that you have a rapid draft drawing, this is solidworks way of handling large complecated drawings, again this should be resolved by hitting the rebuild and following the instructions.

let us know if this solves your problem, if not I have a few other ideas.

demojock...

 

[monge]

Thanks for your response, Yes I have tried all of those sugestions, the rebuilt light will not do, my setting for automatic update off is uncheck, I force rebuilt (CRTL + Q) but nothing will do except to go to the view, right click, properties,go to configuration info and load the model but is not a solution because even that I save the dwg. when i open it again is back to the " detached from model" state. I would like to know of your other sugestions, thanks in advance....Monge
PS.: Not, is not a rapid draft dwg.

 

[Demojock]

Ok, now we start to hit some more interesting questions, are these files just on your local machine, or is there a network involved?

when you open a file in SW over a network it saves a local copy on your machine and sometimes you can accidently "save as" at this stage and get all your links in a muddle.

with the drawing open, click on a view and do a right hand mouse button to activate its properties, this will show you the model information, (file name and location) check this carefully to see that it matches up with where you think it should be, (check in your windows explorer to ensure that this file is there as well)

if everything is where it should be then it starts to get even more interesting, open the drawing up in the SW explorer and do a "find references", again check all links/configurations, etc. if this still doesn't help, drop another reply and I'll see if I can think of any other ideas.

demojock...

 

[monge]

Some info I should have given since the begining of this thread.....
hardware:
Dell comp. w/pentium 4, 1/2 gig of RAM, windows 2000/sp1, nnidia ge force2 gts/ge force2 pro
software:
solidwork 2001/sp9

1. Yes, there is a network and the files are where they should be I verified this by loading the model( when the model is "detached from model" there is not info on the properties box as to where is the model at)

2. yes, windows explorer check is ok(files are there)

3. and Yes, solidwork explorer work just fine it gave me all the references ok.

Thanks again for keeping at it.

Miguel.

 

[BBJT]

I know rapid draft was mentioned right off the bat and you stated that it is not a rapid draft drawing. The only time you should receive the message that you are receiving is in the rapid draft mode. Please give this a shot. Open the drawing in question. Right-click in a view and open the model up. Know toggle back to the drawing. Does it ask if you want to load the model. If it does pick yes and the drawing should update. If it did then some one accedently converted the drawing to rapid draft when opening it up.
If this does not work I personally would send the drawing and model into SolidWorks or to the reseller that you bought the software from.

BBJT

 

[monge]

Thanks...
I open the dwg. (blue frame around it meaning = "detached from model&quot I right click on view and selected open model and the model open just fine, togle back to the dwg. no message as if I want to update the dwg., the blue frame still there and is still detached from model and I right click on view, went to properties box, configuration info said: "detached from model" .

The only way to re-attach the dwg. is by right clicking on a view, got to properties, configuration info, arrow down on your config. and inmidiatly will ask you if you want to load the model, say yes and the model get re-attached with out opening the model....

The weird thing is that is happening to a least 3 people in our department, it happened to me before and with out any explanation or any setting being changed it fixed itself on a particular dwg. the next time I open it, but this one does not want to, I go to keep a close watch on this one and keep you informed If we find a solution to this problem

For now I welcome any sugestion....

Thanks

 

[SBaugh]

Monge,

Have you checked references from the open sub-box?

Try this:

1) Open SW
2) File type .slddrw
3) Pick file "one click" stay inside sub-box.
4) Click References
5) Check to see if it is refering to the part or assembly that you are requesting it update too.
6) If it isn't and or even if it is you can force it to find the model by doing this:

a) Put check mark by the model by clicking the box.
b) Go to the bottom of the sub-menu and click Browse
c) Go to the file folder of the existing model.
d) Ok it and return to sub- box.

7) Make sure "Preview" is the only one checked.
8) Now click Open

Is this drawing a drawing of an assembly or a part?

If this doesn't work for you either let me know I have another Idea I would like to try, but I need to know whether or not this is an assembly or a part.

Hope this helps, Scott Baugh, CSWP
George Koch Sons,LLC
Evansville, IN 47714
sjb@kochllc.com

 

[monge]

wow! Thanks for your input.... but...

You right when I go to the sub-box I click on my file (once) then I check my references, the green check mark is missing, the path is ok but not check mark, so I click on it to check it, so far so good the green check mark is there, I browse to the folder and is ok, go back to the sub box, only preview is checked, click open, the dwg opens with the same problem " unattached from model" I go back to the sub box check the reference box, the green check mark is missing....

for your info this particular dwg. is of an assembly, but it happened to a part dwg. too, the only diference is that for some reason, the part dwg. fix itself after I open it for a few times, do not remember doing nothing special, that is why I'm suspecting solidworks, I don't think we have a corruct file for the same reasons, it does not give me any indication of being corruct,but I will not ruled out either, after I re-attached the model everyhting works just fine, the problems is that you have to re-attached it eveytime.

I would like to try your other ideas, Thanks in advance..

Monge

 

[SBaugh]

Monge,

Idea (1):
This may seem stupid, but I have to try it.

Have tried just making a new drawing of the model?

1) Open the assembly model.
2) Start a new drawing like you normally would.
3) Insert the assembly into the drawing.
4) Save the assembly drawing under whatever name you want & put it in a file folder of your chosing. Note: Before you save it check the reference box at the bottom of the sub-menu and see if it is giving the correct path.
5) Now close everything.

6) Now open your drawing and see if it stayed attached to the model.

I'm curious to know where the drawing is loosing it's reference to the model at. This one may help distinguish what and where the problem exists.

Idea (2):
When your in the drawing that will not reference the model. Tell me, in the Feature Manager Tree (FMT) try right clicking the first item in the list? (Should be the file name) A sub menu shows up tell me what is checked there. This is what is checked in mine

1) Automatic view update
2) Link to external dim text

If niether one of these are checked, turn them on and let me know if that helped

Question(1):
Can you right click a view and open the model?

Question(2):
Can you do the same as Question(1) except go through the FMT Drawing views and open the model?

Is there a possiblility that I could see the files that are causing you such pain?

I'm trying, bear with me. Scott Baugh, CSWP
George Koch Sons,LLC
Evansville, IN 47714
sjb@kochllc.com

 

[monge]

Yes, when I start a new dwg. everything is ok, no problem at all, is that I they allready have some much info. on the bad dwg. that I'm refusing to give it up, besides I would like to get to the bottom of it because it can happen again just like it did before.

Idea 2: I right click on the first item ( file name) and both, automatic view update and link to external dim text are off, so I turn them ON but nothing happened, I tried ctrl + Q ( force rebuilt) nothing, saved and open it again, my view update is on, dim to ext. dim is on, nothing happened still.

Q1. Yes I can right click any view and open the model but the dwg. will not update.

Q2. yes, I can right click any view on FMt an open the model just fine but still my dwg. will not update.

Q3. unfortunately to us, the model and dwg. is propietary, and pattend are summited and pending for this protype and they will not release anything.

Thanks.

Miguel

 

[SBaugh]

No problem, I can understand that! I work for a company like that too.

Well I only have a couple of more suggestions.

1) Talk to your VAR they should have signed a non-disclosure form with your company when you purchased SW. So that they CANNOT disclose any thing about your designs. They may be able to help you better, if they can visualize the problem themselves.

2) I understand not wanting to give up on the drawing that has a bunch of info on it. But you could make a new drawing of your model. If possible open up your other drawing that won't update and try copying some of the info from one sheet to the other (Like notes and stuff like that). Dimensions will have to be redone manually.

I'm afraid to say it, but I think your drawing file has been corrupted somehow. Because there are some good suggestions here in this post that should have worked by now. A lot of the good suggestions are by the first few posters of this thread. I figured they would have had your issue fixed by now, but since those didn't work, I'm leaning towards a corrupt file.

I took some time and went through both the SW help files and the Knowledge Base at SW website without a hit to this problem. So at this point I would talk to your VAR.

I'm at a loss to why this is happening. I apologize for making you go through all of this without a good end result. If I think of anything tonight when I get home I'll post here again. I do hope you or your VAR finds the problem. If you do find the answer please post it because it's bugging me.:-I

Good Luck, Scott Baugh, CSWP
George Koch Sons,LLC
Evansville, IN 47714
sjb@kochllc.com

 

[BBJT]

I agree with Scott Baugh. I worked for a SolidWorks VAR for just over two years(1999 - 2001. I do not recall anything like this ever coming up. Your best bet would be getting the files to your VAR so they can pass them onto SoldiWorks. I have had pretty good success with SolidWorks fixing corrupted files. It will be hard, however, for SoidWorks to determine what is causing this to happen if there is no consistant way of recreating the problem.

Good Luck,

BBJT CSWP

 

[monge]

Thanks to all That responded to this thread, specially Scott baugh, demojok, bbjt, after posting it in another forum and getting almost the same answers regarding the above mensioned problems and looking a the file we determined that in fact was a rapiddraft dwg. the reason that it will open with the unattached model, not that we intended that way, it may be that we unintentionally convert it to rapiddraft with out paying attention ( most likely explanation) or maybe solidworks di it ( less likely).

Any way, before I open the dwg. on the open box it give you the option if you want to load the model, THAT'S telling me is a rapiddraft, because when I hoover on a dwg. that is not rapiddraft, instead of asking me if you want to load the model, it ask you IF you want to convert to a rapiddraft, yet another proof that I'm dealing with a rapiddraft on my original problem.

Someone mention that when loading large assy. dwg. Solidwork will ask you if you want to convert to rapidraft on one those standard looking pop up boxes, and sometime you don't read musch less proofread at all, you just look at the box and click yes, thats probably when it happened so you may want to read those pop up boxes before clicking yes, because there is not going back once your dwg. is converted. you may have to redraw the whole thing over again.

Thaks for all the input.

Monge

 

[BBJT]

Monge,
You make an excellent point about reading the dialog boxes. I had one of our users run into the exact problem the other day. I did not realize that SolidWorks prompted you, when creating a large drawing, to create a RapidDraft until I tried to retrace her steps. I almost made the same mistake by clicking yes before reading the dialog. In my opinion I think the prompt is a bad thing. I immediately sent in an Enhancement Request into SolidWorks to remove this prompt. I recommend everybody that reads this to do the same. I am also talking directly with SolidWorks on this issue.

To remedy the situation we started up a new drawing and copied the views from the rapid draft into our new drawing. It seemed to copy all the views including the balloons just fine. Now the drawing is no longer a rapid draft.

BBJT CSWP