How do I edit an excel sheet to enter so it shows up on a finished drawing? I have a part configuration with about 30 variants (Dim A, Dim B, Dim C, ect) and need my excel sheet on the drawing sheet.
All my prior cad is with Civil3D (autodesk, and my new job is mechanical using SW). Totally lost and the tutorial wasn't much help.
Thanks!
If you're importing the design table into your drawing to show the dimensions of different configurations then my suggestion is to create a new table with a blank row between the SW data. Then you can format the table to display how your would like along with different column names, number formats, etc.
Then, hide all of the rows above the table so all you can see is the version you want to display. On your drawing, insert the design table and it should more or less show what you want. It's a bit frustrating to format this but I've done it in the past.
Thank you so much for this answer. I'll be trying these out at home after hours and am really excited to have found new methods to learn!
One way of doing this is to create a BOM in the drawing sheet and modify column headings so that they pull in your Dim A, Dim B, Dim C, etc data.
1) In your part file I would change the dimension names to reflect what it will show in the table. Example, instead of D1@Sketch1 change it to A@Sketch1 and so on. In File, Properties under the custom tab you would create Property names A, B, C, etc. The Value/Text Expression would just be the dimension you need. You can select the dimension if you have Annotations/Show Feature Dimensions checked.
2) You would need to create a dummy assembly file to show all the configurations of the part. In one assembly configuration, show one instance of your model. This will be used to show the dimensions in the drawing. In another assembly configuration show all the instances of each model configuration. You do this is so that your BOM pulls up all the data for each configuration.
3) In the drawing file you place your assembly file using the assembly configuration with all the part configurations. You can move this drawing view off of the sheet. Create the BOM selecting the model configurations view and modify the headings. Insert another view showing just the one instance of the model and place dimensions on it and change the dimension text for each dimension to show A, B, C, etc.
I've included a zip file containing a part, assembly, and drawing file to show what I have done to do this.
The file version is SolidWorks 2018
Harold Black wrote:
One way of doing this is to create a BOM in the drawing sheet and modify column headings so that they pull in your Dim A, Dim B, Dim C, etc data.
1) In your part file I would change the dimension names to reflect what it will show in the table. Example, instead of D1@Sketch1 change it to A@Sketch1 and so on. In File, Properties under the custom tab you would create Property names A, B, C, etc. The Value/Text Expression would just be the dimension you need. You can select the dimension if you have Annotations/Show Feature Dimensions checked.
2) You would need to create a dummy assembly file to show all the configurations of the part. In one assembly configuration, show one instance of your model. This will be used to show the dimensions in the drawing. In another assembly configuration show all the instances of each model configuration. You do this is so that your BOM pulls up all the data for each configuration.
3) In the drawing file you place your assembly file using the assembly configuration with all the part configurations. You can move this drawing view off of the sheet. Create the BOM selecting the model configurations view and modify the headings. Insert another view showing just the one instance of the model and place dimensions on it and change the dimension text for each dimension to show A, B, C, etc.
I've included a zip file containing a part, assembly, and drawing file to show what I have done to do this.
The file version is SolidWorks 2018
Million thanks for your sample file and detailed explanation. I was just trying to do the same thing.
It was a great help to figure it all.
thank you.
You are welcome
Go to Insert>Tables>Design Table and hide/show ncessary columns/rows as needed. I'm not sure if this is what you were looking to do. The Design Table is also parametrically linked so changes to the model can be made from it. if you require more than 26 rows (I think), save as an Excel 97-2003 table, it allows more rows to be shown.
I think this is closer to what I'm attempting. The person doing my training is swamped in change orders so what I can gather is this. Draw 140 parts, each an edited version/configuration of the last. From the initial parts configuration add/insert design table.
From the ISO drawing of the parent part, click on one of the views (lets say front), this should "activate" the part allowing me to then insert drawing table onto the sheet. I'm sure I've lost a few steps there, but maybe that helps. Thanks!
Steve Make sure your design table is finished in the part, create all of your configurations within the design table as well before inserting.
Steve Make sure your design table is finished in the part, create all of your configurations within the design table as well before inserting.