CAD Forum

I need help trying to figure out if this is possible.

History:
We use SOLIDWORKS 2020 SP5 and PDM Pro.

Our drawing borders are set up to populate automatically, either from the model file properties, or from the drawing file properties. We have trained users that they should not “Edit Sheet Format” and manually change any values on the border.

Our offices in Germany do not allow multiple sheet drawings. They have a certain call out on the drawing border for “type of document”. For example, a single part drawing is called a “-01” document, an exploded view drawing is called a “-20” document, etc. Their drawing files have the normal 8 digit part number and the document type as part of the file name. So there might be multiple drawing files for the same part, for example, 29001568-20.slddrw, 29001568-04.slddrw, & 29001568-05.slddrw. Each drawing is separate and represents a different type of document. In the drawing border, it clearly states the part number and the type of document.

Now to the problem:
We acquired another company in Germany and they have multiple sheet drawings. We are trying to not force them to split their multiple sheet drawings into individual files. To accomplish this, we are thinking that if we can add the “type of document” number to the individual sheets, they would be ok as the multisheet drawing. Each drawing sheet would need to have a different “type of document” number displayed on it.

• We want this “type of document” number to be displayed on the Sheet Format and not on the sheet itself.

• We do not want them to manually change the Sheet Format (if at all possible).

• We cannot use variables from within PDM (because they are assigned to the drawing file, not to the individual sheet).

• We cannot use File Properties within SOLIDWORKS (because they are also assigned to the drawing file, not to the individual sheet).

• Is it possible to have a macro do what we want?

• Can we somehow link a note that is sheet specific?

Help!

Could you attach it to the part/assembly file? as in the configuration specific area?

Then use the proper configuration on the proper sheet?

dpihlaja wrote: ↑Wed Mar 17, 2021 1:18 pm Could you attach it to the part/assembly file? as in the configuration specific area?

Then use the proper configuration on the proper sheet?

Thanks Dan, I thought of that. But unfortunately, the same configuration can be used to create the different type of document. For example, the configuration that is used to create the exploded view drawing (-20) is also the same configuration that would create the "dimensional drawing" (-05).

It is almost like we need to be able to create something that only resides in the drawing file itself and can be controlled by the sheet itself.

My first thought would be using custom view labels. It could be semi-automated (I believe).

mike miller wrote: ↑Wed Mar 17, 2021 2:02 pm My first thought would be using custom view labels. It could be semi-automated (I believe).

We would like to keep this identification on the Sheet Format. I don't think you can put a view label on the Sheet Format because there are no views there.

I'm making some assumption here.

1. You want the document type "number" to show up in the title block.
2. You want this number to be specific to each sheet.

Two ways I can see to do this:
1. Create a sheet format for each document type with that text set. When adding a sheet you pick the sheet format to use.(Some redundancy as you have multiple sheet format files that are nearly identical)

2. Use the "Title block" feature to make that "document ID" and editable field that isn't linked to any custom property. (Really this is no different than modifying the sheet format and editing the text except you control what's can be edited and its a simple double click on the title block (No edit sheet format). Reloading the sheet format resets it to the default value though.)

Thank you @jcapriotti.

Your assumptions are correct.

1. I thought of the multiple sheet formats, but that just gets very redundant. They have 4 different drawing sizes and would need at least 3 different sheet formats per size. I think that is too many sheet formats to control.

2. I will have to look into this one. Thanks.

Another option @VicFrauenfeld is a macro that inserts the document type as text or a block onto the sheet in a standard location. I know it on the sheet and not the sheet format but we do this to insert a part number block and standard notes and tables in drawings. It's one macro but it uses the property editor with buttons for different notes/tables to insert.

I have a couple of ideas. I'll start with the simple one, and ignore the complex one if simple is good enough.

Make a single new drawing template, (not sheet format!) which contains a sheet of every possible purpose where each sheet is already purposed in its sheet format. Name the sheets to easily distinguish them. The sheet with single part drawing already has its suffix hard coded. The sheet with the exploded view drawing already has its suffix populated. Etc.

User makes drawing from part, selects the supertemplate, deletes the sheets which do not apply. You have multi-sheet drawings, with the chosen content types that are left, and all the borders autofilled so you can enforce the don't-touch-that rule.

If a user had to insert a new sheet in the process that was previously deleted, make that whole thing new and independent from the supertemplate, then copy the new sheet into the live document.

To me, this is vaguely similar to having my ConnectionType property pre-populated with SW / NPT / Flange / Compression where 97% of cases only have one which applies. I delete the ones that do not apply because it is easier than typing any of it. It is not a radio button selection list because it can have multiple types. At least you do not ever have multiple types of drawings on the same sheet, I hope.

I think I might have solved my issue.

If we place a note in the Sheet Format called $PRP:"SW-Sheet Name(Sheet Name)", we can then name the sheets the different document types (from outside the Sheet Format like we originally wanted).

Thanks for all the great ideas everyone!

Yep, I'm surprised none of the people suggested that. We use sheet names for our sheet numbers.
This is the easiest way to do this. And depending on circumstances may be the best.
Now, if you want to swap those sheet formats out for existing drawings I have a macro that will do that at:
https://cadforum.net/viewtopic.php?p=606#p606

mattpeneguy wrote: ↑Sun Mar 28, 2021 10:29 am Yep, I'm surprised none of the people suggested that. We use sheet names for our sheet numbers.
This is the easiest way to do this. And depending on circumstances may be the best.

Why wouldn't you use the current sheet / total sheet numbers? Our users have a habit of renaming sheet names depending on the drawing. A sheet may be renamed "Flat pattern" or "QC" or "Mfg layout". Less likely on a plain part drawing though.

I'm definitely not suggesting my workflow for anyone else. We insert our sheets into a larger set of drawings. My drawings may begin at 200 or 220, depending on what type of project it is and how complicated it is. So, I use the sheet names to push the sheet numbers to the titleblocks. If sheets get added before mine, I need a way to shift their numbers. I have a macro that prompts for a starting number and renumbers the sheet names.
There are probably very few people that would do it the way I do, and you are right to question it. But, it works for us.

@mattpeneguy Sounds like you are building a large drawing package with sequencial numbering across all drawings and sheets.

Yes, and the formatting of our sheets has to look the same...I'm kinda good at modifying borders, titleblocks, etc. Our title block is vertical on the right side of the sheet...Did you know tables don't work vertically, and text is awful to work with that way, too?

jcapriotti wrote: ↑Mon Mar 29, 2021 12:12 am Why wouldn't you use the current sheet / total sheet numbers? Our users have a habit of renaming sheet names depending on the drawing. A sheet may be renamed "Flat pattern" or "QC" or "Mfg layout". Less likely on a plain part drawing though.

@jcapriotti We were trying to get each sheet to have a different value placed on the drawing border. This different value was for "document type". For example an exploded view drawing is a "-20" and a drawing for a customer would be a "-18".

For the number of sheets on the drawing, we do use the current sheet / total sheet numbers.