6 Replies Latest reply on Jan 5, 2018 10:51 PM by Rob Edwards

    ? text expression to add an numerical constant

    Dan Aninaru

      Good evening every body,

       

      I intend to get automatically dimensions starting from summary custom (info summary window) toward slddrw sheet. So I created new fields like: length, width and thickness (clicking direct in sheet on concerned dimensions & getting the values, nice !) and I want now to increase them by a numerical constant  value , let say 3/4 inches for each of them, meaning over sized dimensions to be cut before final operation.

       

      Could you tell me the right text expression to be completed in VALUE / TEXT / EXPRESSION ?, so manner to get the right total . You'll better see this, if you open the atachment showing in detail what exactly happen ! I hope this explain you good enough my trouble, and will be easier to you to come with the answer. I tried following the same rule as in Excell using F4 touch bringing $$ (and keep this numerical constant fixed, but is not the case,  not programming (Visual Basic ?)). May be Solidwork use another ?! (by the way, wich one ?)

       

      Thanks again and enjoy the new year 2018, comming soon

      ps:  Hope my written english (not my most fluent language I know) is understandable.

       

      Dan Aninaru

        • Re: ? text expression to add an numerical constant
          Rob Edwards

          Hi Dan

           

          You can use Global Variables in equations to calculate your new fields

          You are not limited to using global variables, you could create any variable to represent your data

          eg an offset plane

           

          Then you can add these to your file properties..

          To add a dimension, show it in the graphics area and click it, if using a global var, its even easier as they are already  in the drop down menu

          Hope that helps

            • Re: ? text expression to add an numerical constant
              Dan Aninaru

              Mr. Edward,

              I do not want to skip, some information you bring me with global variables & equations, but I can't see how add that an equation in this

              field shown below. The over size 3/4 is not realy material streched it is just like looking like. I see your last picture showing equation symbol in model and this look like out of model. Iis this true ? (seem to be bigger)

               

              I tried this unsuccessfully. But I started after from this window

               

              Finally I got it, (LENGTH instead LEGTH, and click on 18 13 /16 inch dimensioned on part, in first field) but still do not know how to bring in the Slddrw file as below.  I make a text box clicking into it

              to get some equation anywhere...............Shoud be added 4 3/4 (4+3/4) or 18 13 /16 +3/4

               

              Thank again,

            • Re: ? text expression to add an numerical constant
              Kevin Chandler

              Hello,

               

              Rob Edwards correctly replied to your post: you must use global variables to compute values.

              Custom properties don't have the addition ability shown in your image,so the addition you entered is treated as text and is quoted as typed.

               

              Also, Mr. Edwards reply depends on your underlying file for the drawing being a multiple body part file.

              If it's an assembly file, the dimensions you will need to reference (as shown above) will be in the individual part files (and not in the assembly file)

              If it is an assembly file, you will have to create global variables (in the assembly) using the "Measure" option (see 2017 SOLIDWORKS Help - Global Variables) to create the required dimensions so the drawing can see the linked properties (as shown above).

               

              But considering this post's image and your other post: Can I print in one file from individually slddrw ? following pages numbering ! , I think a different approach would be better for your situation.

              • Since you are combining part details within an assembly, when you add a constant value to a dimension that spans multiple parts:
                • To which part does the added material belong?
                • How much of the extra material goes to each part?
                • For example, the 25-3/4" overall height dimension applies to the "SOLIDE CERISIER" and the "FINGER GRIP".
                  • Where will the extra 3/4" go?
              • Also, I don't recommend adding the same amount of extra material for all dimensions, especially for the thickness.
                • This example doubles the thickness, which would added (I think) too much extra stock cost and machining time.
              • Also, how much material to add for each part's fabrication (and any subassemblies) depends on the processes used and their quality (tolerances) the process can maintain and on the final product's required quality (tolerances).

               

              Before you go much further:

              • I suggest consulting your fabrication people to see what's required where and when.
                • Also ask them if my "suggested approach" below would be benefical for the product (and for your company).
              • Check with your purchasing people to see what material sizes are readily available and at what costs.

               

              My suggested approach:

              • Create each part as its own part file and create a drawing file just for this part
                Using "SOLIDE CERISIER" as an example:
                • Create an extrude as the first operation and make this extrude the size of the stock required for this part.
                  • The stock thickness should be what's commercially available or the thickness you're actually purchasing
                • Using extrude cut, "remove" the material as it would be machined
                  • For "SOLIDE CERISIER", this means:
                    • Cutting the tongue
                    • Leaving extra material on the face opposite of the tongue if you later machine the assembly to the 32-3/4" final width
                    • Leaving extra material on the length if you later machine the assembly to the 25-3/4" final height
                    • The stock thickness should include extra material if the thickness is later modified
                      • The extra amount depends on the process to achieve the final thickness (planing? sanding?)
                  • Create a configuration of this extrude (this will be used later on this part's drawing)
                • Save this as another configuration.
                • Create a drawing from this part.
                • Add views using both configurations with text labeling each view as STOCK PART and FINAL PART.
                  • Dimension both views
              • Create the "FINGER GRIP" and the large panel (without the band) the same way as above, adding material that's required for fabrication to achieve the final quality,
              • Create an assembly of the parts and mate them as required
                • Save this as a configuration as it's oversized and machining will be needed for the product's final dimensions
                • Using extrude cut, "remove" the extra material to the product's final size.
                • As was done for the parts, create a dedicated drawing with both configurations shown, labeled and dimensioned.
                • Note: this assembly may be for just the panel and two "SOLIDE CERISIER", since these may need to be assembled first and their top edge machined for a clean mounting face for the "FINGER GRIP".
                  • If so, then this 3 peice assembly is then inserted into another assembly along with the "FINGER GRIP" and mated.
                    • With configurations and drawing as above.
                  • The extra material is then removed from the bottom edge to achieve the final height.
              • The last assembly will also show the crossed band, which would be modelled into the last assembly since it affects all parts at final location and size.
                • Finishing would also be noted on the last assembly drawing.

               

              This may seem like extra effort, but:

              • It frees up time elsewhere
              • It makes for more complete drawings, reducing potential errors and scrap.
              • With dimensioned stock drawings, you can inspect cut stock and reject out of tolerance stock before adding increased costs with added work to future scrap.
              • With each part documented, you can route each part independent of the others (other than maintaining scheduling).
              • With each part documented, you can track inventory levels, costs and delivery times for each for a truer assessment of the situation.
              • Allows you to easily send any part out of house for outsourced fabrication (if justified by the finances)
                • Can help compress a tight delivery schedule
                • Can avoid adding capital expenditures or labor training if current capabilities aren't alreadt in-house
              • You can outsource just the cut stock, a fabricated part or a subassembly.
              • You can reuse parts in other assemblies.
              • Allows you to outsource to a vendor better skilled at certain processes (labor, machinery, expertise, cost) where needed.
              • For out of tolerance parts (final part, subassembly or cut stock), you have a drawing to rely upon for remedying the situation (especially when outsourced).
              • Each part and assembly can be revised and documented independent of the others.
              • With more information, there is less guessing and interpolation.
                • This will lower variance, which automatically raises quality.

               

              Please excuse the long discourse.

              Just my thoughts from woodworking days gone past.

               

              And again, Happy New Year to you and your family,

               

              Kevin

                • Re: ? text expression to add an numerical constant
                  Dan Aninaru

                  Hello again,

                  Thanks so have to use global variables to compute values. Realy I didn't try yet.

                   

                  Concerning my pictures (doors and drawers) with clears and rough dimensions, instead to bw drawn individually to keep more tight with production and stock, quality etc I want to tell you my example with the front door & drawers at the time in one slddrw file, was too "complex" for you in my Discussion opened: ? text expression to add an numerical constant. "I took the bad one", instead taking a simple one. Anyway your explanations, bring me manny ideas just in case I will have that kind of processing in production. In woodworking industries some time we do not keep tracking so tight on parts, but I recognize some time we should do so manner.

                  Let you now you do not spend time, bringing me many ideas in this context and I aperciate this.

                  I like your suggested approach leaving extra materials. The operators they do this by heart, reading the assembly (drawer and doors drawing)

                  I like this a lot you say, but the reality you know ......

                  • You can outsource just the cut stock, a fabricated part or a subassembly.
                  • You can reuse parts in other assemblies.
                  • Allows you to outsource to a vendor better skilled at certain processes (labor, machinery, expertise, cost) where needed.
                  • For out of tolerance parts (final part, subassembly or cut stock), you have a drawing to rely upon for remedying the situation (especially when outsourced).
                  • Each part and assembly can be revised and documented independent of the others.
                  • With more information, there is less guessing and interpolation.
                    • This will lower variance, which automatically raises quality.

                  We let the variance going up where statistical by the machines and first of all starting by the humain beeing (thinking) wich is the first variance that cause and start problems (the machines less).

                   

                  Mr.  Kevin thank you for your thoughts from woodworking you already was in, may be.

                   

                  Dan user

                • Re: ? text expression to add an numerical constant
                  Rob Edwards

                  Another way to do this, that is a lot less work once you have set it up is to use an equation in a BOM

                  and then save the BOM as a template.  No need for anything else then

                  2016 SOLIDWORKS Help - Table Equation Editor