51 Replies Latest reply on Apr 2, 2015 2:02 PM by John Stoltzfus

    Solidworks Drawing Format Issues

    Tyler Murray

      I have spent days trying to set up a decent drawing format and researching how to do things with the drawing templates and table templates etc all to no avail... I don't get why Solidworks has made setting up a default drawing format so difficult but sure wish they would figure out a way to fix it in the future.

       

      Here are my biggest complaints that I can't find a solution to.

       

      1) You can't add a BOM table to sheet template. I understand this is because there is no part/assembly referenced but is it really that hard to have a blank BOM in a template that is populated once the part/assembly is added to the drawing?

       

      2) Revision tables unlike BOM's can be added but only with partial success. What I would like is for it to put the revision table in place and have revision 1 with a description "For Review" and then set the date as the date the drawing was created. So far I have only found it possible to get one or the other, I can create it so that it has the first revision listed with the description I want but I can't find a way to make the date automatic so have resorted to leaving it blank but that isn't a real solution... Other option is to input blank table format and then click to add revision but this requires the description to be entered every time on every sheet... 

       

      3) Then when you click to add a new sheet to the drawing it again has no tables so you have to do everything again... You can add them in and have it linked to first page but it never anchors properly(always defaults to not anchored and even if you remember to click anchor it then defaults to top right anchor which you can't even change without first creating table and then going back in and changing it after...).

       

      4) If you try to get around this by copying the original sheet and pasting it then everything looks good but the revision table isn't linked to the first sheet anymore for some reason...

       

      5) It would be great to be able to create a list of common notes and then easily be able to choose which ones you want to have on the drawing. I have heard this is possible with autocad but have never used it. The best we have found is to have a list of notes on the sheet template which works ok but a guy spends a lot of time deleting unneeded notes or retyping which then leads to discrepancies between drawings(notes typed differently every time).

       

      All in all these may seem like little trivial issues but in the end it can often lead to spending more time fiddling with drawing formats then actually creating the drawing... Whereas if it was possible to do the above things then all a guy would have to do is create a few different base templates and pick the right one for the situation and then start annotating.

       

      If anyone knows any ways to solve some of the above issues I would love to hear them. Otherwise hopefully SW can improve on this in the future since imo this is one of the biggest weaknesses right now.

        • Re: Solidworks Drawing Format Issues
          Bernie Daraz

          have you looked into Custom Properties? Everything you have mentioned can be covered by that. But I should add with the exception of a BOM. How would you know how many columns and rows it should have? Maybe you are making assemblies of just one or two pieces but there's no way for me to know that from your post.

           

          Most places I have been only place a revision table on the first sheet of a drawing. I have a custom property file that allows me to select notes as well as material types and finishes to place on the drawing. In my case I don't edit the field of the drawing. SolidWorks offers a lot of drawing automation. There are standard date properties for "drawing creation date". For a changed date and others you could use a property to show the current date.

           

          In my case I had been misspelling anodize on many drawings. Once I made that a property, anytime in the future that I reopen that drawing it will automatically correct itself. Now that I select it from a drop down (along with my other finishes) I will never misspell it again. One of these days I'll make the 'anodize' finishes only appear when I use an aluminum alloy capable of being anodized.

           

          Sharing a custom property file is a little difficult, as good as it may be the drawings it is used on must be so configured as well.

            • Re: Solidworks Drawing Format Issues
              Tyler Murray

              We need the revision table on all sheets or I guess at least something set up that calls the current revision and date from the main sheet. The reasons for this is that we make complicated parts that have individual pieces that we send to different machine shops but instead of making the part a complicated assembly of small pieces we build it all as one and then use drawing sheets to go over details of each small piece then only send the applicable drawing to the shop making it. In this case each drawing needs this information on it hence why I am trying to figure out how to stream line this. The revision table works fine if you manually enter it on each sheet and link to original but it just takes a lot of time to do this when I think it should be fairly easy for solidworks to make it automatic(works halfway already).

               

              As for the drawing creation date how does one reference this property? I have tried searching what it is called and it very well might exist but I have been unable to find it. If you are referring to entering custom properties and just calling those then yes I know how to do that but it would take less time to just enter it on table(problem is this date often doesn't get updated because we are always rushed).

                • Re: Solidworks Drawing Format Issues
                  John Stoltzfus

                  Tyler,

                   

                  A lot of good questions....

                   

                  I have setup my custom property builder to handle most of the issues you mention.  Here I also use multiple sheets in a drawing file and I have setup my own revision table, because there could be one or more components changing in an assembly, so I want those revisions to reflect at the part level and also at the main assembly level.  Prior to doing a new design I save a new custom property builder so that I keep the input as minimal as possible, mostly the only items that I need to add is Machine designation and description...  Most of the other stuff is automatically filled out in the drawing.

                   

                  I agree with Bernie, almost all your issues revolves around custom properties - once you learn to set it up and use it, you'll wonder how you did without it.

                   

                  I also have different sheet formats for assemblies and parts, and you can also add additional sheet formats to match your needs, then when you insert a new part or assembly, just right click the drawing and load another format, those sheets could have different notes attached to it...

                   

                  As for the BOM that is a small issue to deal with, I also have 3 different BOM's that I deal with here, depending on the information that I need to pull off of for our ECN's

                    • Re: Solidworks Drawing Format Issues
                      Tyler Murray

                      John,

                       

                      I haven't used the custom property builder but if I understand it right it is just another way to set up a part's properties which I already do. I do this by creating a new part and then going into file/properties and changing the part/assembly properties. I created my part and assembly formats to have a list of properties already programmed in so all I have to do is enter the data(title, description, material, etc). This way my drawing formats/boms etc are all automatically populated via linked data.

                       

                      I could do this for the revision date but the problem is that I don't want the revision date linked to the parts or assembly properties but rather the drawing itself and I would like it to automatically update instead of having to manually enter this date. In other words when I create the new drawing for a part I would like the revision table to have the first line already in place(which is possible) with the current date of the drawing being made(it is possible to link the current date but then it changes every time you open it).

                       

                      What I would ultimately like to achieve is a drawing template/format that when I finish making a part I can go to file/make drawing from part, choose my preferred drawing format for that part, insert views, insert new sheets as necessary to fully define part and have all these sheets(including first sheet) already have all the bom's and revisions tables in place and defined properly.

                       

                      If a guy could do this I figure it would save me about 1/3-1/2 the time I currently spend on making drawings. Most of our parts are very simple and the drawings take little time to make, that is why all this time spent on manual table creation bothers me.

                        • Re: Solidworks Drawing Format Issues
                          John Stoltzfus

                          Not sure I understand what you want then....

                           

                          Do you fill out the custom properties from here ........??

                           

                           

                          If you do then your spending a lot of time going through each line.........

                           

                          I don't understand why you wouldn't want the revision going with the part.. For me I want to know what changed, when and where and our ECN backs up the why..

                           

                          It used to take me a long time as well doing the drawings towards what it does now, search for Custom Property Tab Builder, once you use it (like other things), you'll never go back, lol

                           

                          Based on your questions and your end goal, you're on the right mind set in trying to speed up the process and yes SolidWorks does have tools in place to assist with some of these wants, it's just we need to do our homework and apply what we learn and all will be well.

                           

                          I have set up my Custom Property Tab Builder to minimize the input required, most projects I just type in the description and the rest is pre-input and saved then I just need to choose the proper file..

                            • Re: Solidworks Drawing Format Issues
                              Tyler Murray

                              John,

                               

                              Yes that is the page I use. I have it set up though so all the property names are already there(included in part and assembly templates) as well as any formulas for formula driven properties(like material grade and mass). All I have to enter is the data that would be required no matter which way I do it.

                               

                              The only property that I currently need/am looking for is a solidworks generated property referring to when a drawing file was created. I would use this on the revision table for a standard revision 0. The type of property I am looking for would be similar to $PRP:"SW-Short Date" (which gives you the current date) but that doesn't update each time I open the file.

                               

                              Other then that I have no issues with properties. My main issue is with the incapability to add revision and bom tables to the template/format. Something I don't think any of us can fix unfortunately and something that in this day and age(read computer programming ability) I feel is unacceptable.

                               

                              Thanks all for the 2 ideas about drawing notes though, I will play with both and see if either works for us.

                                • Re: Solidworks Drawing Format Issues
                                  John Stoltzfus

                                  Ok - You would benefit greatly in learning to use the Custom Property Tab Builder. 

                                   

                                  The picture below shows a simple assembly and I can edit all the components properties while in the assembly, including the assembly properties. There is no need to open, change, save and close every part, all you do is either select the part in the feature manager tree or in the assembly view and go to the right click on the property tab and edit all the info required - nice, easy and quick..

                                   

                                  That portion usually had me way up in arms, 100 parts, 100 times to open, 100 times to change, 100 times to save, 100 times to rebuild and 100 times to save, and hopefully I didn't forget something

                                   

                              • Re: Solidworks Drawing Format Issues
                                Brian McEwen

                                I don't have a solution but just wanted to show my support for your idea, those things could be better.  Some little things you be able to put in a macro - such as add the current date, maybe create a BOM for the first sheet.

                                 

                                I certainly agree we should be able to put in an empty BOM on the template (and specify which empty view to link it to).

                                 

                                If your projects are very similar you may be able to use DriverWorksXpress to start your drawings, but that is just speculation.

                                 

                                For #5 we use a combo of standard notes on the template, and Design Library annotations for the less common notes.

                        • Re: Solidworks Drawing Format Issues
                          Glenn Schroeder

                          #1.  You asked "is it really that hard to have a blank BOM in a template that is populated once the part/assembly is added to the drawing?".  I'd ask is it really that hard to insert a BOM after you've inserted the drawing view?

                           

                          #5.  It is possible, and there are at least two ways to do it.  The one I prefer is to save the Note as a Style.  Open a new drawing and create a Note with the attributes you want (text, Layer, font, etc.).  With the Note highlighted, click on the Add or Update a Style icon.  That will let you name the note, and in the future it will be available to select from the drop-down when you activate the Note function.  You can save as many notes as you want.  When you're finished saving all the notes you'll need for a particular type of drawing, then save the drawing template.  If the notes aren't saved in the drawing template then they will only be saved for the one drawing.  If you have multiple drawing templates, as many people do, this allows you to have different Styles saved as needed for each one.

                           

                          You can even save notes that are linked to custom properties or cut list properties, but for these you may need to insert a drawing view to attach the note to, then save the Style, then delete the drawing view before saving the drawing template.  You can later attach them to any drawing view and they will reflect the properties of that model (you may need to click on a model edge instead of just the drawing view in general when inserting the note for it to pick up the property, even if the Note doesn't have a leader.)

                            • Re: Solidworks Drawing Format Issues
                              Tyler Murray

                              1) Adding a single BOM doesn't take long but say adding 6 boms to a drawing set when each piece on that set only has a handful of dimensions it quickly takes longer to add BOM's and revision tables then it does to actually create the drawing. 

                               

                              In reply to Bernie, having a BOM table with no part reference doesn't affect the number of rows hence why a guy can set up a BOM table format that works for different sizes of assemblies etc. All solidworks needs to do is set it up so the BOM references all parts/assembly on the drawing sheet and then sit blank if no part is referenced. Seems pretty easy to me but maybe there is some unknown reason as to why they haven't done this. If not hopefully they will change it as it would reduce one step in making these drawings.

                               

                              5)  I will try the style method and see how that works. Thanks

                                • Re: Solidworks Drawing Format Issues
                                  Bernie Daraz

                                  I will agree with you though as Glen mentions, it easy as pie. Not his exact words. Of course our format is set in stone so I can't investigate this. If you were to set up a format for three or four different row counts what would happen when you forget a part in an assembly, let's say a screw. The row will print but it will not be outlined. That could be a minor problem but how would others interpret that? How would you handle blanks lines. Then in the worst case, what happens when you leave and the next place doesn't have what you want and you can't change their practices.

                                   

                                  Don't misunderstand my comments, I'm not trying to insult you. It is situations like these that make people look for solutions to problems.

                                   

                                  A macro might be a solution.

                                    • Re: Solidworks Drawing Format Issues
                                      Tyler Murray

                                      Bernie,

                                       

                                      I must not be understanding you properly or you have your BOM's set up differently. BOM row counts are variable and do not have to be defined in setting up a BOM template. A BOM template simply states the column properties to display then solidworks automatically populates rows depending on number of parts/assemblies in the model. Solidworks already does this well and I already have 3 different BOM templates defined depending on the situation.

                                       

                                      My quirk/issue is that you have to manually add a BOM to every sheet whereas I feel it should be possible to add a blank BOM to the sheet template/format so you don't have to do this.

                                        • Re: Solidworks Drawing Format Issues
                                          Bernie Daraz

                                          I don't set row numbers, I think I may have been misunderstood. The component count defines the BOM row count and that is automatic. Though since a lot of the older parts I reuse do not have properties entered I display the BOM on the assembly, that 'forces' me to enter the required data into properties. The company has set standards for drawing data and practices but wasn't aware automation could handle most of the input.

                                    • Re: Solidworks Drawing Format Issues
                                      Dwight Livingston

                                      Glenn

                                       

                                      We looked at Styles but decided to use the Design Library instead. We set up a couple of notes folders on our server. We can drag a note there to save it. We have quite a library there now, and we don't have to worry about what notes go in what template.

                                       

                                      The only down side we found was that it couldn't handle GD&T frames.

                                       

                                      Dwight

                                      • Re: Solidworks Drawing Format Issues
                                        Wendy Mark

                                        1) I agree with you, No, it's not hard.  However, I agree with Tyler too; it is non-value-added, time-consuming steps for something that is automatic in other CAD programs, and so should logically be able to be automatic in SW too.  Everybody in our company has expressed frustration with this, since we had "assembly drawing templates" in our previous CAD program, and now can't find a way to get them again.

                                      • Re: Solidworks Drawing Format Issues
                                        Mike Pogue

                                        I think some of these are good points, but some are caused by trying to do things non-standard.

                                         

                                        I can help you with number 5, at least. I've seen many ways to do this, but the best and easiest is to have every note on the drawing template--not the sheet format; you should never edit the sheet format during normal use. There is no retyping, only deleting. No errors, no fuss no muss.

                                         

                                        • Re: Solidworks Drawing Format Issues
                                          Kelvin Lamport
                                          5) It would be great to be able to create a list of common notes and then easily be able to choose which ones you want to have on the drawing. I have heard this is possible with autocad but have never used it. The best we have found is to have a list of notes on the sheet template which works ok but a guy spends a lot of time deleting unneeded notes or retyping which then leads to discrepancies between drawings(notes typed differently every time).

                                          Try the CommonNotes macro from Lenny's SolidWorks Resources

                                            • Re: Solidworks Drawing Format Issues
                                              Aaron Torberg

                                                   You can save annotations (notes in this case) to the design library under annotations.  You can even save them as lists so that once you add one dragging and dropping another on top of it creates a single formatted list style annotation (numbered, like in the image posted by Mike).  In the image Mike Pogue posted you could save each of those numbered notes as a separate annotation and just combine them as needed by dragging and dropping.  Is this what you want?

                                            • Re: Solidworks Drawing Format Issues
                                              Tyler Murray

                                              I figured there was a solidworks property for created date. Not sure why I couldn't find it before but for others interested it is `SW-Created Date` (go figure...). You can use it as `SW-Created Date(Short Date)` if you only want the date(enter in table under equation). At least now my Revision 0 row will populate correctly.

                                               

                                              Now if only a guy could add the bom and/or revision table to the sheet format so they would appear each time you create a new sheet/drawing...

                                              • Re: Solidworks Drawing Format Issues
                                                Tyler Murray

                                                Unfortunately I spoke to soon and like too many other instances what should work doesn't... The SW-Created Date property does work in both new and old files but if you put it into a revision table format then it stays as a formula but reads the day you created the format... If you click the field and press enter it will update which would make you think clicking rebuild would solve the problem but of course it does not for some unknown reason...

                                                 

                                                Just another little nuisance I guess I have to live with. Becoming more and more obvious this program is not meant to be automated and that manual input for each and every detail on a drawing is the only solution... A little disappointing imo considering how much this software costs...

                                                  • Re: Solidworks Drawing Format Issues
                                                    Glenn Schroeder

                                                    Tyler Murray wrote:

                                                     

                                                    Just another little nuisance I guess I have to live with. Becoming more and more obvious this program is not meant to be automated and that manual input for each and every detail on a drawing is the only solution... A little disappointing imo considering how much this software costs...

                                                    Tyler,

                                                     

                                                    With all respect, there are many drawings created every day with SolidWorks, with a great deal of the process automated, and certainly not with "manual input for each and every detail".  I'm sorry that it doesn't do everything you think it should the way you think it should, but what does?

                                                      • Re: Solidworks Drawing Format Issues
                                                        Tyler Murray

                                                        Glenn,

                                                         

                                                        Solidworks is a powerful tool and it can do a lot of things but there are no excuses for programming errors like this and I come across little issues like this to often hence why I am trying to bring attention to them by posting them here.

                                                         

                                                        Maybe I am doing something wrong but so far no one here has been able to provide any work arounds for how to include a bom and revision table in a drawing format, something that to me seems rather elementary since most drawings require both....

                                                          • Re: Solidworks Drawing Format Issues
                                                            Glenn Schroeder

                                                            Tyler,

                                                             

                                                            You aren't doing anything wrong, and I'm certainly not trying to start a fight.  I don't use Revision tables so I can't address that.  I do use BOM's.  Not on every project, but maybe on 1/3 of them.  In my opinion the process of inserting them into a drawing is already pretty simple, so I'm puzzled over why you're so adamant that they should be a part of a drawing template or sheet format, but if it's that important to you, then by all means submit an Enhancement Request, and/or create an Idea for it here next fall.

                                                             

                                                            Glenn

                                                      • Re: Solidworks Drawing Format Issues
                                                        Tyler Murray

                                                        Ok I kind of found a work around regarding BOMs. One of the main problems is that we have always used a BOM table even for parts. Since a part is only ever a single line on a BOM it finally dawned on me to just create my own property driven table instead of using a modified BOM table... Realistically it is the same thing with the same properties but you can put the basic table on drawing template whereas you can't put a BOM on the template for whatever reason.

                                                         

                                                        This only works for the first sheet of a drawing though. Does anyone know if/how a guy can set solidworks up so that all new sheets use both the sheet format(easy) and drawing template(not so easy?).

                                                         

                                                        Glenn, I will submit a few enhancement requests. When you look for help it points you to this forum hence why I started here.

                                                         

                                                        Thanks

                                                          • Re: Solidworks Drawing Format Issues
                                                            Aaron Torberg

                                                            My first though on this is that you will have a difficult time with ballooning your assemblies based on a table that is not a BOM table - I have never done this so maybe its not that hard but this is probably not standard practice.

                                                            • Re: Solidworks Drawing Format Issues
                                                              Glenn Schroeder

                                                              Tyler Murray wrote:

                                                               

                                                              This only works for the first sheet of a drawing though. Does anyone know if/how a guy can set solidworks up so that all new sheets use both the sheet format(easy) and drawing template(not so easy?).

                                                               

                                                              Glenn, I will submit a few enhancement requests. When you look for help it points you to this forum hence why I started here.

                                                               

                                                               

                                                              Tyler,

                                                               

                                                              I'd like to help, but I'm not exactly sure what you mean by "if/how a guy can set solidworks up so that all new sheets use both the sheet format(easy) and drawing template(not so easy?)".  The properties controlled by the drawing template remain unchanged for the entire drawing, regardless of how many sheets it has.  #2 here: Frequently Asked Forum Questions  may help.  If not, please elaborate.

                                                               

                                                              And this is the best place to start when you need help with something.  If it can't be done the way you want, or you can't get the help you need here, then it may be time for an Enhancement Request.

                                                               

                                                              Glenn

                                                              • Re: Solidworks Drawing Format Issues
                                                                Brian McEwen

                                                                That is a good idea to use a general table.  We use a general table for our Revision table actually. (there are lots of posts about ways to set up revision tables, some of them are in the EPDM forums, but many of the ideas can be used without PDM)

                                                                 

                                                                You can't add tables to the sheet format, and the sheet format is what is used for additional sheets...

                                                                If you are only talking about a single row BOM for the 2nd sheet (and other additional sheets), then you can sketch the table into the sheet format using lines. Then place text linked to properties. That doesn't sound great to me but it is the only way I can think of to have a BOM-like-table appear when you insert a 2nd sheet. I guess you could save it all as a block, to make it easier to delete if you had a different case. 

                                                                 

                                                                There is now (2014 and possibly earlier) a setting in Document Properties>>Drawing Sheets>>Sheet format for new sheets and select Use different sheet format.  For us this does not work, it can't find the sheet format I select. But if it works it should add a sheet using whatever sheet format you specify. 

                                                              • Re: Solidworks Drawing Format Issues
                                                                John Stoltzfus

                                                                Tyler,

                                                                 

                                                                LOL - I was on the "Assembly" track of mind - I know what you need, I have done it for years, (I don't have a copy here, send me a message with your information and I can send it to you sometime mid next week, got some days away), and, yes it is a very simple fix on your end, you need to go in the edit sheet mode and draw some lines where the information needs to be shown.  The template that I have, the information is shown along the top side of your sheet, including part number, description, material size, material, qty needed and if it gets laser cut or not...

                                                                 

                                                                Sorry about that, I should have asked, or maybe you did mention it before, but............

                                                                 

                                                                And...... (edit)

                                                                 

                                                                You save this format as a different template then you can choose which layout you want to use, I had about 4 different ways that I needed to show information

                                                                • Re: Solidworks Drawing Format Issues
                                                                  Mark Greenwell

                                                                  Hi Tyler,

                                                                   

                                                                   

                                                                  If you only have single part per drawing why use a BOM.

                                                                   

                                                                   

                                                                  Why not just set up the drawing to carry the part info, all mine populate automatically from the custom properties of a part.

                                                                   

                                                                  This way I can have as many sheets as I like and all will be populated.

                                                                   

                                                                  part.PNG

                                                                   

                                                                  Or have I totally missed your point.

                                                                   

                                                                  Thanks

                                                                   

                                                                  Mark (SolidWorks 2015 sp2.1)

                                                                    • Re: Solidworks Drawing Format Issues
                                                                      John Stoltzfus

                                                                      That's what I was talking about

                                                                        • Re: Solidworks Drawing Format Issues
                                                                          Mark Greenwell

                                                                          Hi John,

                                                                           

                                                                          I thought every one did it this way when you have one part per drawing.

                                                                           

                                                                          I was taught this way, A GA drawing shows all the assemblies (In a phase) together on one drawing.

                                                                          An assembly drawing was a drawing with all the parts on one drawing therefore you would need a BOM.

                                                                          A part (or component) drawing should always be one part per drawing and therefore a BOM was not necessary. Information would be shown in the title block.

                                                                          The only time we would need a general table added to a part drawing would be if the part was used over multiple assemblies. The general table would have the assembly number and qty required added.

                                                                           

                                                                          Thanks

                                                                           

                                                                          Mark

                                                                            • Re: Solidworks Drawing Format Issues
                                                                              John Stoltzfus

                                                                              Right on Mark - there are different ways companies want their information shown and I know what threw everybody under the Bus here was the word "BOM"

                                                                              What Tyler needs and I think wants is what you have shown.

                                                                                • Re: Solidworks Drawing Format Issues
                                                                                  Brian McEwen

                                                                                  We'll see what Tyler says, but I don't think it is quite that simple John. The single part on a drawing may be just one case. 

                                                                                    • Re: Solidworks Drawing Format Issues
                                                                                      John Stoltzfus

                                                                                      Could be Brian - The only issue is if he wants more than one part per drawing - that would be a problem.  I don't know of anyone personally that does multiple parts on one sheet, however I know there are applications where its nice to have the relating parts all in one view. 

                                                                                      • Re: Solidworks Drawing Format Issues
                                                                                        Tyler Murray

                                                                                        Brian and others,

                                                                                         

                                                                                        This is effectively what I did by creating my custom table. As you guys mentioned I should just draw the table so that it can be included in my format and then it will work on each sheet. Doing the same for a revision table would probably solve that issue as well but am I correct in saying it would only be possible to show the current revision information and that it would have to be run via part properties(instead of clicking revision table which is handy). Or is there a different trick some of you use to get around this?

                                                                                         

                                                                                        This solution will only work for simple parts. For multibody parts and assemblies I will have to use the BOM/cutlist tables and manually insert them but at least I should be able to cut down on my part drawing times which is the main hassle.

                                                                                         

                                                                                        Thanks

                                                                                          • Re: Solidworks Drawing Format Issues
                                                                                            John Stoltzfus

                                                                                            Thanks for starting this discussion - there was a lot shared and I was glad to see some of the answers myself, there are other ways of doing things, most times I'm stuck in my own time capsule and not realizing things do change...

                                                                                             

                                                                                            Each revision is based on a part - sub assembly - or assembly, so here I need every page to carry it's own revision table, however like you mentioned you can't use the SW revision table in a multiple sheet file.  Some of my drawing files have over 100 tabs and I want to go from tab to tab rather than opening up a 100 files.  So I created my own revision table and revision properties that they required here, so when I do a new product release we have different steps of revisions based on the different reviews and adjustments, therefore it is really easy going to the next step in the revisions if it's a blanket revision, meaning all the components get the same rev number/letter, I use Task Scheduler and within a few minutes I can bump everything to the next level.

                                                                                             

                                                                                            If there is a particular component that needs adjustment then only that part is updated and a new rev released, after that you have to pick individual parts in the Task Scheduler so you don't change each one if there are different levels of revs in the multiple tab file.... Therefore everyone of my sheets either assembly or parts need to have the revision table