REQUEST: Please review proposed file system

[Mechomatic]

Hello all-

If you've got a moment, I'd appreciate your input on a change I'm proposing for my company's system of saving Solidworks models and drawings. We run SolidWorks 2012 x64 SP5.0.

Our file server has a "SolidWorks Drawings" ("SWxDwgs") folder and a "Job Files" folder (just sticking to the pertinent info, here). SWxDwgs contains solid models, assemblies, and SWx drawings, along with occasional .pdf or .dwg versions of the .slddrw files on an "as needed" basis. Job Files contains the customer specific models and drawings for when we make specific configurations of equipment for a customer and also for us to have reference models down the road so we know what components/equipment a specific customer received. Currently, revisions (general and customer specific) are handled by: Save a Copy of the model under revision file name (part#-rev-type.SLDxxx), then making a new drawing for the revised part (since references to the original drawing were broken with the save-as-copy change). It's basically a big mess where we're experiencing solid model/assy bloat, never really making a revision to a drawing- just making a whole new drawing, and wasting a whole lot of time.

The system change I'd like feedback on is as follows:

SWxDwgs folder contains models and drawings for each component and assembly. When a revision is to be made, a new configuration in the model is created with the changes. The drawing is opened, the referenced configuration in the views is changed, and the drawing is then saved with the new revision number. As old versions are phased out, their drawings can be saved as a PDF and sent to an archive folder and the old configuration can be deleted from the solid model/assy. This way the most recent version of the model and drawing is always available in the SWxDwgs folder without the assembly file bloat (# of files) and we don't have to keep making drawings from scratch for every revision to a model.

In the Job Files folder, the customer specific configurations must be kept for an indeterminate amount of time. To do so, I plan to save the top level assembly/assemblies as Parasolid Binary files (.x_b) to the job files folder. This way any changes to the models used in the SWxDwgs folder (as time and revisions pass) do not affect the reference model saved to the job files folder. Drawings submitted for production will be saved as PDF files to the job files folder, as well, so that -again- no changes elsewhere affect what is saved as reference information in the job files folder. When we get customer specific requirements for a job, the configuration(s) required will be applied to the SWxDwgs folder files as revision configurations (so they are available at a later date if we get the same requirement down the road).
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Does this sound like a suitable method to keep us from having to keep making drawings from scratch for each revision, while maintaining reference models/drawings for job files? Thank you for taking the time to wade through this post, and I sincerely appreciate any feedback, whether it's a "thumbs up" or constructive criticism.

 

[EEnd]

It sounds like you would get a good ROI on upgrading to PDMWorks Workgroup. It does a reasonably good job of managing revisions. If that is not possible, I think your existing strategy with some modifications would be better than your proposed one. Using configurations to manage revisions seems like it will lead to substantial grief.

First, you do not need to recreate your drawings. There are several ways around starting from scratch. Here are the two that I have used the most.

One is to open the drawing, save it with the new revision name, leave the drawing open and open the component file, save it with the new revision name and tell SW that you want to update references in open files. This should get you new drawing file linked to a new component file.

Another is to make copies of both the drawing and component with the new revision names in Window's explorer. Then go into SW and start to open the new drawing. With the drawing selected in the open dialog, click on the references button. This will open a dialog that will let you link the new drawing to the new component file.

Both of these strategies can be used to on assemblies as well as drawings. SolidWorks Explorer can also be used to copy files and manage references. There is also the pack-and-go feature which also has features for copying files and updating their names.


Eric

 

[Mechomatic]

"One is to open the drawing, save it with the new revision name, leave the drawing open and open the component file, save it with the new revision name and tell SW that you want to update references in open files. This should get you new drawing file linked to a new component file."

That does sound much better, thank you! Keeps the work and number of steps down without adding complexity or copying components all over the place.

Will doing this update the parent assembly, though, with the revised part, or will I have to go back and replace components in the parent assembly (breaking any drawing balloons and dimensions in the parent assy drawing attached to the old revision of the subassembly)?

 

[Mechomatic]

Where is the option to "update references in open files?" I just tried saving a drawing, resaving it as a new name, then opening the model, and resaving it as the new name, but I didn't see an option or dialog box to update references.

http://www.linkedin.com/in/wapratesi

 

[CorBlimeyLimey]

Will doing this update the parent assembly

Any assemblies or drawings open at the time the Save as function is used, will be updated if they reference the part being saved.

 

[CorBlimeyLimey]

Where is the option to "update references in open files?"

The References button is at the bottom-centre of the Open dialogue box ... just above the File name field.

 

[EEnd]

When you do the save as of the component, SW will (unless you told it not to show you again) display a popup with the following message (circa 2012):

<file name> is being referenced by other open documents. "Save As" will replace these references with the new name. Check "Save As Copy" in the "Save As" dialog if you wish to maintain existing references.

For what you are doing, you will want to leave "Save as copy" unchecked. Leaving this unchecked is what I meant by updating open files. It has been a while since I did this so I was unsure about when / how you made that distinction.

To make a copy of a component and update it in both the drawing and an assembly(s), have both the drawing and the assembly(s) open when you do the save as. I think you will want to work in a top down fashion. If the highest level assembly has a drawing, open its drawing and it. Save as the drawing to the new revision. Save as the assembly to the new revision. Save and close the assembly drawing. Open one of the revised components and its drawing. Save as its drawing. Save as the component. Save and close the drawing. Save the parent assembly. Repeat until you have worked your way through the tree. I have not used it for this purpose, but I pack and go may let you do something similar with fewer steps.

If you discover that you did not have something open when you did the save as on one of its references, you can open it, using the references button to link it to the new file name. You will then want to save or save as the referencing document.

Eric

 

[Mechomatic]

I'll be playing with this next week to make sure I have the method (and consequences for messing up) down pat before moving on actual implementation.

Thank you both, so much, for your help!

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