4 Replies Latest reply on May 31, 2018 8:04 AM by Ben Siddall

    Excel driven tables in drawings

    Ben Siddall



      I'm wanting to produce a set of drawings based on a large quantity of standard parts I have. Basically I have created a sketch within a drawing of the basic part and added dimensions to this labelled A, B, C etc but without a value. I have created a table below the drawing in a drawing view so I can now type the information into the table with the correct dimensions for that part, essentially the values for A, B and C. Each of the parts I have are the exact same apart from the dimensions and I don't want to draw these out using a configuration table as not all the dimensions are accurate and work out properly meaning I would encounter a lot of errors. I don't need any part files, just drawings referring to the dimensions.


      What I would like to do is to type all of the dimensions out for A B and C dimensions and the name of each different version of the part into an excel spreadsheet. Is there then a way to copy this information for each variation of the part into separate solid works drawing files? Basically I have all of the dimensions for all of these parts (approximately 1000 of them) on old sketches and drawings but they all rely on the same dimensions, I'm wanting to get all of these onto solid works drawing files and then exported as PDF's in the quickest way possible. If there is a way of me typing these into a spreadsheet and then letting solid works generate separate drawings then that would be ideal.


      At present I have created a drawing template with the sketch and dimensions in and a separate table below linked to file properties within the drawing, I then type these values in and it copies them into the table for me to export as a PDF but it is still taking a while and does mean me manually creating a new drawing file for each one of these.


      If anyone could shed any light on this then that would be greatly appreciated. Thank you.

        • Re: Excel driven tables in drawings
          Peter Brinkhuis

          I suggest you look into using a Design Table. If you already have a thousand configurations, SolidWorks can put their data in the table. If you only have the data elsewhere, you can create a thousand configurations by adding the dimensions do the design table manually.


          Doing all of this by hand doesn't sound like fun though, even data entry will takes hours or days. Maybe we can help you by developing a macro or an add-in, if you do this kind of work often that sounds like a must.


          If you want to create tens to hundreds of drawings quickly, our drawing automation tool Drew can help Drew | CAD Booster

            • Re: Excel driven tables in drawings
              Ben Siddall

              I thought about using a design table with configurations but not all of these parts actually work out, and each one would need individually tweaking. Due to this I would rather not have these as parts but just separate drawings instead. Thank you.

                • Re: Excel driven tables in drawings
                  Dennis Dohogne

                  Ben Siddall wrote:

                  I thought about using a design table with configurations but not all of these parts actually work out, and each one would need individually tweaking. Due to this I would rather not have these as parts but just separate drawings instead. Thank you.



                  You came here for some advice and Peter gave you some good advice.  What you are describing is a table drawing, where one configuration is physically shown, but its dimensions are listed as A, B, C, etc., and are then shown in a table, usually along with a part number.  This is easy to do.  Just show one of the configurations with dimensions, change the default <DIM> of the table dimensions to the table letters A, B, C, respectively, and then import the Design Table (from saving it out/exporting it from the part file) or just copy the contents of the DT to a temporary Excel file and then copy that into the General Table on your drawing.


                  Here is a quick and dirty example:


                  HOWEVER, your statement that not all the parts would work out and that some would need individual tweaking is rather disturbing.  That is all the more reason to put them into a Design Table - for the ease of creating the parts and verifying the geometry.  Individual tweaking is then easy and those tweak parameters do not have to show up in the DT.


                  Table drawings are pretty easy, but the parts need to lend themselves to such tabulated dimensions, i.e., the differences in the parts should only be in those tabulated dimensions and not in additional tweaking; for that you should just give each part its own drawing.


                  Now, let''s say you really want each part to have its own drawing, but the parts are in a DT and there is tweaking.  This is perfectly fine.  An easy way to keep from having to re-do a lot of work is to take one of the more complicated configurations and fully define it with dimensions on a drawing.  Now, copy that sheet either to a new drawing file or as another sheet in that same drawing file.  Then you change the configuration of that new sheet to a different config.  The dimensions will update their values so that is very nice.  Let's say this configuration has different tweaking so now some of the old dimensions are left dangling.  They will be a different color and easy to spot so you just delete them and then you can add in any new tweak dimensions that are unique to this configuration.


                  I'm trying to be helpful here, but please understand my alarm from your statement that not all the configs would work out.  The whole point of 3D CAD systems is to verify on the computer that all parts DO work out.

                    • Re: Excel driven tables in drawings
                      Ben Siddall

                      Apologies I should make myself more clear. Essentially I have around 1000 old drawings / sketches of components that are mostly the same apart from the main few dimensions which differ. A lot of these dimensions are from customers in the past who have measured these components by hand with a tape measure. The parts are just basic pieces of sheet metal rolled to a curve and the dimensions are either the radius, length around the curve, length across the curve and the height. Some of the old drawings / sketches have for example the radius, the height and the length around the curve which in solidworks would produce an overconstrained model as only two of these are needed.

                      I have produced a drawing file with a pre set table specifying all the available dimensions and a sketch of a random curve with every dimension labelled (A) (B) (C) etc to reference to the values in the table. The sketch is just what I have drawn by hand within a drawing view and is only for reference.

                      Although a design table would be ideal, I'm wanting a different drawing file for each one of the different configurations which I can save to a pdf. Each drawing needs to have as much information on as possible but obviously I would not be able to produce physical parts for these as they would be overconstrained due to all the dimensions. They don't always work out due to customers measuring them by hand, which is why we tweak things when we come to producing them. There is a good chance a lot of these will not be produced for many years to come and it would be too long of a process to individually go through all of the models to make sure it works out with the dimensions provided. All I want to do is to copy all the information I have for these parts into separate drawings all following the same format using the companies standard template.

                      I mentioned excel as I was hoping there was some sort of way of generating multiple drawings based on the values in an excel spreadsheet. I'm not sure if something such as Drew cad booster could do something like this. It would be much easier for me to input all the information I have for these in a spreadsheet with a colum for the part name and one for dimension A for example and then me go though and type this all into a big spreadsheet. I was then hoping there is some sort of tool to automatically transfer all this information into solidworks drawing files using my pre-made template and then I would go and export each one to a pdf.

                      Its hard work and I knew it would be a problem but I would save me manually creating a new drawing file for each drawing I'm wanting to produce and inputting all the information in that way.