I want to make a Table of Contents that has the name of the sheets linked to notes in a table on the cover page of my drawings.
So far, I have to manually type in all the sheet names from the "rectangle area" into the notes in the "square area" I don't know anything about macros, so if there is another way to do it please let me know.
Not the answer you're looking for, but...
I also use multiple drawing sheets and I have 4 or more cover sheets, however we don't want them to be counted in the total sheet number so I run the attached macro that was written by Leon Wurr.
Are all your parts listed or just assemblies? I would create a Custom Property that is called "Drawing Title" and in the certain assemblies you add that note or description which I would collect in a custom Custom BOM.
Yeah, all that does is give Sheet "X" of "X" I need somethings that pulls the names of individual sheets and makes a stacked list of them. I will say I feel a lot better after using his macro. I will look for more macros to try and solve my problem.
Thank You John.
Even if you use a macro somewhere you'll still need to "Input" the data, that's why I would lean more to creating a Custom Property and creating a new Bill Of Material. The important part is to type only once, surely there is someone that would know how to read the sheet tabs.....
I also have a macro that I run that changes the "Default" configuration name to the file name, (assemblies & parts), and then I run another macro to change all my sheet tabs to the configuration name in the part or assembly, that's doing it in reverse of what you want...
Maybe Viktor Bovzdarenko from #Task would know and it would be a great macro to add to their list....
Matthew Gray, This is an interesting request. If after a short time you don't get a good answer then please add this to the Top Ten list. https://forum.solidworks.com/content?filterID=all~objecttype~objecttype%5Bidea%5D&sortKey=all~objecttype~objecttype%5Bid…
I don't know how to do that either. lol
This problem should be something as simple as making a note and linking it to a certain Sheet Name. Any more than that and it is not in-line with the whole Solidworks Idea. Older more complicated cad programs have this ability and one day so will we...until then I just have to shoot up a flare and hope it gets seen.
@ John Stoltzfus, I want to thank you for all your input thus far. You have gotten me closer to my objective than anyone else and maybe the answer is out there I just need to keep looking.
See following post. It gets you 80% there. Search forum for "api sheetname" and you'll get plenty hits for a routine that traverses all drawing sheets and retrieves the sheet names.
How to list all the configurations of an assembly in a Solidworks drawing parametrically?
Matthew, Try this link SOLIDWORKS World 2017 Top Ten List
If you have trouble getting in then try contacting Matthew Lorono or Richard Doyle
Matthew,
Where are the titles of the different sheets coming from? Are they custom properties of the assemblies on the individual sheets?
I name the sheets, Cover General layout, Bill of Material, etc., I have a "table" drawn on my Cover sheet with the DWG NO. Drawing Title and REV of specific sheet. I will attach a .slddrw file for y'all to open and look at and play with. I just want to make the individual notes under DRAWING TITLE to correspond with the SHEET NAME it references. That way I can add a sheet if needed and the note on the Drawing Index updates accordingly.
Here is the Drawing Sheets
For starters you can link the tab name and insert that into your drawing header
By creating a note and selecting the link icon
Then in the property drop down menu select "Sheet Name"
So we can read the tabs and we can write to the tabs, but to get the information from the tab into a table or BOM will be the sticker.....
Yes...I have already done what you have said. It's the stickier part I am stumped on. getting those same notes all on the cover page.
Do you use Custom Property Tab Builder?
I have
Ok do you put different top level assemblies in one drawing sheet? Do you use different configurations?
I will put my main assembly for the entire project on the cover page. Usually just one ISO view. The general layout wil have a few views with overalls and a few specific dims, as well as part call outs. Then bill of materials "for parts only". I do have some configured parts but only two or three of them. I usually have 100 different parts and several sub assemblies and one main assembly.
Here is what I would try -
Then run the attached Macro that changes the Tab Names to match the Configuration Name - then link the Tab Name to your drawing format to insert that name "Sheet Name", in the Title Block as you show -
Then Setup a custom BOM that Links the Sheet Name to a column along with the latest Rev and assembly/part number
I know it's not what you're looking for, but I would use it rather then typing out a table every time..
The following will read drawing sheet names and insert those into the drawing custom properties. A table or note could be linked to those properties at that point.
'preconditions
' SW drawing is open
'post condtions
' drawing sheet names added to drawing document properties list
'
Sub main()
Dim swApp As Object
Dim swSheet As SldWorks.Sheet
Dim swDraw As SldWorks.DrawingDoc
Dim vSheetNames As Variant
Dim i As Long
Dim swCustPropMgr As SldWorks.CustomPropertyManager
Set swApp = Application.SldWorks
Set swDraw = swApp.ActiveDoc
Set swSheet = swDraw.GetCurrentSheet
Set swCustPropMgr = swDraw.Extension.CustomPropertyManager("")
vSheetNames = swDraw.GetSheetNames
'delete exising properties 0 through 10
For i = 0 To 10
swCustPropMgr.Delete i
Next i
'repopulate properties 0 through -- with sheet names
For i = 0 To UBound(vSheetNames)
swDraw.ActivateSheet (vSheetNames(i))
Set swSheet = swDraw.GetCurrentSheet
retval = swDraw.AddCustomInfo2(i, swCustomInfoText, vSheetNames(i))
Next i
swDraw.ActivateSheet (vSheetNames(0))
MsgBox ("Complete")
End Sub
Awesome John -
A question -
What is this deleting the Sheet Name??
If I have over a 100 pages should I change the 10 to 200?
Not quite sure how to handle that:
The macro adds properties numbered 0 through # of sheets.
It assumes the user didn't already have those as entries for something else.
And on a second go around using the macro, it would need to either overwrite or delete those pre existing "0 through # of sheets" entries somehow.
So yes change.
Same thought here...a lot of my Drawing Packages have 10-15 pages.
This returns the property value as numbers, which is ok - and I can get it to populate - If it can read the sheet tab, it should also read the description and rev at the same time, is that possible, or make it that we can change those values, this could be good...
To get it to populate I made a list in excel starting $PRP:"0" all the way to $PRP"50" and then I added a note in the drawing sheet and Cut & Pasted the Excel column
Try this combination.
Using original drawing supplied, properties are populated with sheet tab names (0 through 16, no tab = "N/A"), and table on first sheet is linked to those properties. You could customize to suite as far as drawing template and table size, number of sheets etc.
Try this combination.
Using original drawing supplied, properties are populated with sheet tab names (0 through 16, no tab = "N/A"), and table on first sheet is linked to those properties. You could customize to suite as far as drawing template and table size, number of sheets etc.