- Add a design table to the part, and show that (there are some tricks to getting it formatted correctly.
- add a SW table and start typing.
- make an excel table and insert it into the drawing.
- make an excel table and copy paste the values into a SW table on the drawing.
only option 1 is linked to the dims in your configurations.
Thanks Jeremy. Right now I'm placing a view of each config in the drawing and using a BOM table with each config. Then hiding all the views except for the one to dimension. Then cleaning up each table to make it appear as one table. And the dims in the table are linked. This is a total work around, but it sounds like it's not any more work than your #1. Having the dims linked, as in my example and your #1 is the way to go.
Definitely sounds like you are doing more work than you would be just utilizing the design table. You can use it as just a reference table rather than driving your actual configurations.
Create a tab instance for each configuration and link a single column to display your variable dimension and you're done.
config. / description / dimension "x"
01 - short - 5in
02 - medium - 7.5in
"Create a tab instance" What's a tab instance?
Sorry, just a line in the table for each respective configuration. We refer to them as "Tabs" here for multiple variations of the same part/material.
Basically the "01, 02" column in my original post example.
Newell or anyone else, I created a design table from a part that already had configurations. I let it auto-create. I attempted to place that in my drawing by going to insert, tables, design tables. I got an error message saying the table is corrupt. I didn't do anything other than let it auto-create. Do you know why I'm getting this error message?
Try inserting a blank table. It is probably struggling to identify all the different variables to put in the table when using auto-create (which you don't want anyway).
Manually enter the information in a format similar to my first example, leaving the first row empty. Then just link one column to the desired property by entering the value in the header (1st row) and hide that row.
Hello Newell or anyone else, I created a blank table and inserted it into the drawing and still getting the design table is corrupt and cannot be inserted into the drawing message. Any ideas what's causing this? The table whether created from a blank or auto-create, seems to be created without any issues.
I'm running MS Excel 2016 MSO version
Thanks for the thread, that was the problem! That was an issue back in 2011 and still exists today, why am I not surprised:(
For what it worth, when I create a tabulated drawing (which I don't do often) I eliminate the configurations and do it with an assembly and a custom BOM. The model often starts as a configured part but they are saved out as separate files to maintain our one file per part number rule and to allow it to work properly with some automation associated with EPDM. An assembly is created that includes all of the models and a drawing of that assembly is created as the tabulated drawing. The overall process looks like this:
- Create a part model for one of the parts to be listed on the tabulated drawing.
- Click on File...Properties to open the Custom Properties dialog.
- Click on <Type a new property> and enter the text 'A', including the single quotes.
- Click in the Value/Text Expression column.
- In the feature tree, click the feature that has the dimension that needs to be tabulated. If necessary, move the Custom Properties dialog to one side, or to your second monitor so that you can see the feature tree and the model.
- In the SOLIDWORKS graphics area, select the dimension to be tabulated. The dimension name (e.g.
"D1@Boss-Extrude1@Part1.SLDPRT") should appear in the Custom Properties dialog.
- Repeat steps 3 through 7 for any other tabulated dimensions, using other property names such as 'B' and 'C'.
- Click OK in the Custom Properties dialog.
- Perform a Save As or Save As Copy of the model for each item that will appear in your tabulated drawing.
- In each model, change the tabulated dimensions as necessary.
- Create a new assembly model and insert each of the tabulated item models into the assembly.
- Hide all but one of the models in the assembly.
- Save the assembly.
- Create a new drawing from the assembly.
- Dimension the drawing as normal, but for the tabulated dimensions override the dimension text with the custom property name defined in step 3 above.
The next few steps rely on a custom BOM template we made for tabualted drawings. It simply has a columns linked to the custom properties defined in steps 3 through 7 above.
16. Select a drawing view and Click Insert...Table...Bill of Materials.
17. Click the Star button in the Table Template area of the property manager.
18. Select the TABULATED DRAWING template.
19. Click OK and place the table on the drawing. It should already be populated with your tabulated item information. The table will respect the units defined in your model. For example, if you want to have fractional inches for one of your tabulated dimensions, simply override the dimension display in the model to use fractional inches.
20. The default template includes only one tabulated dimension column. If you need more, insert a new column in the table, make sure Column Type is set to Custom Property and select your custom property (e.g. 'B') from the drop down list.
21. Save your drawing.
Thanks Jim for the input. We have a ton of tabulated autocad drawings that we're converting to SW. The SW configuration feature seems to be well suited for this very purpose and saves on a ton of individual files. It seems like your method defeats this purpose, but maybe I'm missing something here?
it comes down to a couple of points
- are you using a PDM system? does that PDM system allow different configurations to have different revs (SW PDM does not out of the box)?
- do you currently have different revs for the different part numbers in one table, and/or want that option in the future?
Jim Sculley specifically said that have a rule of one file per part number. so that is their method. we also have tabulated part drawings and use SW PDM pro, but do not have that rule, so we use configurations. (our rule is 1 drawing per part/assembly).