How can I make an assy drawing remember it belongs to an 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.

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.

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.

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 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.

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).