One of my assembly drawings keeps getting disconnected from the assembly. When I open the assy, then click the feature tree to open the drawing associated with the assy, it pops up a box in the correct folder asking to choose a file. I choose it, save it, close it and when I reopen it and try to open the drawing it pops up the file dialog again.
How can I make the drawing remember it's associated to the assy?
Are both files located in the same folder? I've had issues if they aren't.
Also are both file names the same, again I've had some issues when they weren't the same.
Yes and no. File name for the assy and assy drawing are below.
Label Fixture for 75-2177-02.SLDASM
51-0112-01 Assy.SLDDRW
Are you saying they need to be the same?
Matt, to add to what Peter has already mentioned ...
We do a lot of part drawings that come from assemblies or are cavity feature in an assembly that create a specific part. When working with this type of situation where the assembly may not be directly related to the part/parts in question we will place a model view of the assembly in the drawing off to the side of the drawing sheet. This ties the assembly itself directly to the drawing but it does not print due to not being on the sheet. This way the assembly and all associated part files get checked in when we've completed our drawings.
I don't know if that's your issue or not but I hope it's helpful all the same. That is the only situation I've come across that an assembly would not be checked in with one of our drawings if it should have been associated.
Yes. Same name, and both reside in the same folder.
It really shouldn't be called "Open associated drawings"...it should be called "open drawing of same name", because that is what it is actually doing.
Don't believe me...?
Make a drawing of a completely different part, but name the drawing "Label Fixture for 75-2177-02.slddrw" and save it in the same folder as the Label Fixture for 75-2177-02.sldasm.
Now close everything and just open the Label Fixture for 75-2177-02.sldasm. Now go into the tree and "open associated drawings"...
TaDaaa!!!
Try it and see. Make them both the same name in the same folder.
You have a drawing with the same name, but they are not associated.
You need to associate the model. Open the drawing and associated the model to it.
Assy References:
John Pesaturo, I don't have a PDM vault here so does this still apply?
Peter Kennedy, I saved the assy as the same name as the drawing and sure enough it opened the drawing. I have 2 other label fixtures constructed the same way and they both keep the associations to the drawing even with a different name. Methinks there are multiple ways of doing this (associating drawings with parts/assy) and not all different methods have the same coding. That means Doug Seibel is also largely correct in that this is not file associativity, it is file-name associativity.
I'm confused with this statement,
I have 2 other label fixtures constructed the same way and they both keep the associations to the drawing even with a different name. Methinks there are multiple ways of doing this (associating drawings with parts/assy) and not all different methods have the same coding.
are you staying you have two other files that when you select open drawing the open one with a different name?
Even with PDM professional it only works if the file names are exactly the same and they are in the same folder.
I think that the best answer I can give you is to update your search paths.........system options file locations....search paths. there are many options on the pull down folder.....look threw the list and update the ones that you thing are necessary so that SolidWorks will find your drawing when you tell it to open from the part or assembly. I usually do not open drawings that way...I would rather find the drawing and then open the assembly threw the drawing. I also like a custom property in my parts and assemblies that will tell me what the drawing # is for that file. The best thing is to try and keep the files in the same folders but that is not necessary to reorder all your folders....I have parts and assemblies on one mapped drive on the server and another drive that is just for all the drawings. I have no problems with the file loosing the references.
one more thing about setting the search folders...make sure that you have the one that you want it to look at or for first. I had set this up t find files before and added the hard drive as the top one and it kept finding files on my computer instead of the official ones that were saved to the server, another little pain to deal with.
hope this helps.
Matt,
As most people here recommended, the names must be EXACTLY the same. Even an empty space at the end of the file name would cause issue of linking between them
I thought the entire point of a PDM is to keep track of such references. If you are losing the up references, PDM is not set up well for your company. Though even then you have to go to the PDM vault and look at the 'where used' tab, they don't just show up on the find references function inside an assembly or part.
What program are yall using with the linking issues like that.....I have had a few because of some bad file management...but I have totally different part # names and drawing # names and have not had the issue of disconnected linking....then again I'm on sw 2014 if this is an issue in 2017 someone please let me know before we upgrade....
Well, I was going to say I have two other un-related fixtures that do not show that behavior, but I misspoke. One of them does have the same assy name, and the other does not but it keeps opening the drawing that DOES match the file name. So yes, the file name does have to match in the assy and the drawing.
I am currently using SW 2016, and I thought the way it is suppose to work, especially without a PDM vault is like this;
If you make an assembly, and make a drawing with that assembly, then save both files while each is open, the connections between them should be saved. UNLESS you then go into the file tree and move the files around and/or re-name them. This can happen when you use Window Explorer, or start saving parts and assemblies in different places without having the parent drawing open and re-saved as well.
Also, drawings look to assemblies and parts for their data, but parts and assembles don't actually look to drawings for data, so are not usually referencing them in any way. In other words it is a one-way street.
-In other words, you can go to a drawing and do a find ref (or down reference), and find out all the parts and assemblies used in that drawing. But when you do it from the part/assembly level, the drawing isn't really used to make the assembly/part and finding up references is difficult.
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Without a PDM, best way to find the drawing file that parts and assemblies are used in is to start up SolidWorks Explorer and do a 'where used' search on everything. Yeah, that can take several minutes per search.
Pro-tip; Generally it's a good practice to have a 'top level' drawing, and use that when your looking for all the assemblies and parts used in a project. And if you need more than one drawing for a project, keep them all in one folder or at least using the same number with diffrent extensions so they are all right next to each other in the file lists. It really helps to keep track of everything on a project, rather than trying to find everything from a the assembly level and looking for drawings.
If files are in the PDM, names can be different between the 2D dwg and 3d modesl and under PDM control; however, soon you checkout to your local drive, then it get issue
Try this
1) in the Vault, rename 2D dwg so it's different from its associated 3D model file name. Check files ref. they are still linked
2) check both out to your local drive and close the 2 dwg and open the dwg again from the 3D model. you'll get error message that the 2D dwg never exist until you rename the 2d Dwg again to match exactly wit the 3D model file name. If you miss just one empty space in the file name, Sw still asking for the 2dwg
the open drawing from part / assy command inside of SW has nothing to do with PDM and it knows nothing of the file references in PDM. it is just a macro that someone wrote way back that looks in the folder the file was opened from for a drawing of the same name. the part / assy file has NO knowledge of where it is used. it only looks down (assy knows its sub-assys and parts, drawings know its parts / assys).
Jeremiah Feist is correct. Steven Mills the OP was asking about the open drawing tool accessed by rmb in the feature tree. This is totally unrelated to references. Though I do think a comparable button should be available from the PDM tree where references are used instead.
There is a lot of discussion in this thread related to references and not what Matt Finley was asking about. Be carful reading this and extrapolating or coming to conclusions.
Grant
I posted a reply, but then deleted it, because I misread your question.
The correct answer is: stop using that method. Hit the "R" key (recently opened files) and open it from there. It helps to pin it down (in the recently opened files) if you are infrequently visiting the file.
Dan
I get the impression that a lot of people are responding to the question, without actually understanding the question.
The issue that Matt Finley is having is when he uses the "Open Drawing" RMB option from within the feature tree.
If you open a part or an assembly, and RMB (right mouse button) while your mouse is in the feature tree on the top of the tree, you will get the RMB pop-up option to "open drawing". What Solidworks is doing when you click on that, is it is simply looking for a drawing with the exact same name as the part or assembly. It is NOT looking for a drawing that is actually associated with the part or assembly...it is ONLY looking for a drawing with the EXACT same name.
I have attached a few files. 2 part files and 2 drawing files.
Part file "BALL" is a ball-shaped part. Drawing file "BOX" is the drawing for the ball-shaped part.
Part file "BOX" is a box-shaped part. Drawing file "BALL" is the drawing for the box-shaped part.
Open up just ONE of the part files. In the feature tree, right-click at the top of the feature tree...this should pop up an option to "open drawing...click on "open drawing".
Notice that it opened the drawing that had the same name...not the drawing for the part.
The problem that Matt Finney is experiencing is NOT a loss of association (which is what he was under the impression was happening).
Doug Seibel, I was completely in the dark about how this worked for many years. Funny how perception really can be reality until the perception changes. Thanks for all the help gentle mans.
Yea, I was one of those that misread the question. But, in all reality, the method of always putting the files in the same folder isn't that convenient. That limits you in two ways: where you put your files and the name of the drawing. That's why I never got used to opening my drawings that way.
But, many companies work that way, they put all the files in the same folders and use the same assy/part/dwg name. We do it where I work, but most companies I worked for in the past, didn't do it that way.
Dan
No I understood the question, which is why I did the lecture on how assembly and drawings files actually associate with each other above. Along with tips of keeping things organized when you have a lot of files.
Doug Seibel wrote:
I get the impression that a lot of people are responding to the question, without actually understanding the question.
The issue that Matt Finley is having is when he uses the "Open Drawing" RMB option from within the feature tree.
If you open a part or an assembly, and RMB (right mouse button) while your mouse is in the feature tree on the top of the tree, you will get the RMB pop-up option to "open drawing". What Solidworks is doing when you click on that, is it is simply looking for a drawing with the exact same name as the part or assembly. It is NOT looking for a drawing that is actually associated with the part or assembly...it is ONLY looking for a drawing with the EXACT same name.
Doug is correct, but I would like to add that it is looking for this drawing in the same directory as the assembly.
Also, this is a one-sided situation, i.e., this is true for opening the drawing from the part or assembly - the drawing must be of the same name and in the same directory. However, the converse is not true. If you open a drawing first it knows what and where its part or assembly is (unless it was moved since the last save of the drawing). I am not recommending this practice, just clarifying the requirements for the connections. Knowing this can be handy in the event you open the part or assembly and cannot get to the drawing. If you were to instead open the drawing and it properly shows its guts you can simply look at Find References to see where everything is located and what it is called. Perhaps something got put in the wrong place or was misnamed. So long as you can find the drawing and it opens properly you can figure this out and do whatever is necessary to put it the way you want.
The pdm issue is now becoming a little clearer....moving the files does cause a detach.....but keeping the same name for the part-assembly and the drawing.....still does not make sense to me. I would have a smart part #, to a dumb part # that parts and assemblies are name by. Then I have another system that would generate a drawing #....and I am not seeing the problems that you guys say that you are having,......there must be something up with the settings in the PDM or SolidWorks that is causing this,.to happen. Cause I can name my weldment part the chicken house base framing.....do an assembly where I add some sheet metal parts or plywood siding...not really a big difference there till you start building....then call the 5 sheet drawing design 1 chicken pen. so that I know what the heck it is when I get around to looking at it again.
The logic I am getting is that if the files linked together have to have the same name....what do you do with you parts that you put into an assembly do you rename each part to the top level assembly name....with a ref #. the reference between a part and assembly should be no different than that of the assembly and the drawing...or the drawing and the part.....
I still say there is a solution in the file locations settings.....or that there could be a bigger network issue going on where drives or folders are get changed somehow. that will cause problems too. even if you happen to change the name of a folder and put it right back....there can be issues with the files in those folders loosing links.
Are both files located in the same folder? I've had issues if they aren't.
Also are both file names the same, again I've had some issues when they weren't the same.