22 Replies Latest reply on May 4, 2017 5:44 PM by Robert Millot

    Component Equation Won't Evaluate to 0?

    Robert Millot

      Hello,

       

      I'm using an equation to drive a sketch dimension that will sometimes be 0".  When the equation evaluates to 0", I get the following error message:

      "The equations evaluates to a value that lies outside the modeler resolution."

      Is this for real?  Can I not have a value of 0" for a distance dimension and drive it with an equation?

      For context, the value I'm driving is the pitch height of a part above the top plane, which will sometime be zeroed out and sometimes have a positive value:

       

      I'm not really looking for an alternative solution here; I just want to know if you truly cannot drive a part dimension with equations if it's going to be zeroed out.  This will come up again and again in my industry.

       

      Thanks,

       

      Bob

        • Re: Component Equation Won't Evaluate to 0?
          John Stoltzfus

          I wouldn't want it too, because SW has been known to flip dimensions and then you'll end up with a negative number instead.  Not sure of where you're getting the dimensions from, but what I would do is either offset a Plane by a small amount or add a sketch line that hangs out over and dimension from either of those options, that way your dimension never goes to Zero and therefore no chance of the dimension being stuck or flipping..

          • Re: Component Equation Won't Evaluate to 0?
            Bernie Daraz

            I believe there are some Logic values that can be used in equations such as IF. You might want to investigate that further through the Help files. I have no use for this right now but apparently you do.

            • Re: Component Equation Won't Evaluate to 0?
              Robert Millot

              Thank you for the replies.  Coming from Pro/E, negative (non-flipping) and zeroed out dimensions all seem so fundamental to me; I hope SW developers will one day take care of this problem.

               

              Bob

                • Re: Component Equation Won't Evaluate to 0?
                  Bernie Daraz

                  My first exposure to Pro-E was a customer request for paperless manufacturing on one project. We were given a computer and Pro-E to cooperate in the request. It was between us and another manufacturer. I remember back then the class project was a 'system' driven 'bottle' where we had to design a 'volume driven' bottle to hold a certain amount of liquid. I was 'thrilled' to see that we weren't learning any of the basic but thrown right into this, my first exposure to parametric CAD. Of course my thoughts at the time (2002 ?) were filled with comments (read expletives!) that I won't post here.

                   

                  My question to the OP would be, do you think it was a good 'move' to SW or would you rather be back?

                    • Re: Component Equation Won't Evaluate to 0?
                      Robert Millot

                      There are things I like and dislike about both software packages.  From what I've seen so far, Pro/E is definitely the more powerful program; however, my task is to head up the migration of our current model library from Pro/E to SolidWorks, and I'm trying to retain as much functionality in the process as I can.  It's hard to speculate about the company's reasoning behind the software switch (cheaper? easier to use?), but of course most of the engineers are griping and grumbling about having to learn a new program.  We were using WildFire 3.0, so we definitely need an update in either case.

                      Here is my list of the Pros and Cons of SolidWorks compared to Pro/E so far:

                      SW Pros:

                      1.  3D Sketching (Although I'm sure this is available in Creo by now).

                      2.  Configurations (Although I think Pro/E has a similar function with "Family Tables")

                      3.  Sheet Metal Flange Propagation

                      4.  More Robust Sheet Metal Bend Position Options

                      5.  "Offset from Surface" distance command option

                      6.  Drawing Package is Easier:  Specifically Sections Views and Auto Assembly Balloon Cleanup

                      7.  Ability to "Push" and "Pull" Equations:  From Assembly to Part or Part to Assembly.

                      8.  "Offset Entities" command will cap the ends of the offsets.

                      9.  Crashing a Feature Does Not Halt the Model

                       

                      SW Cons:

                      1.  Cannot Copy and Paste Mitre Flanges

                      2.  Cannot do Sheet Metal Surface Rips

                      3.  No Auto Sketch Relations in Sketch Mode (Except Vertical and Horizontal)

                      4.  The Drawing Does Not Copy when you Copy the Part or Assembly

                      5.  No Complex Cuts in Sheet Metal

                      6.  Suppressing a Part Driven by an Assembly Equation Blows Up the Model (This one was really frustrating)

                      7.  String Variables cannot be created (Useful for bulk assigning Materials and Gauges).

                      8.  Sheet Metal Conversions Are Not as Robust

                      9.  Negative Dimensions Cannot Be Entered and Dimension Vector is Inconsistent (Part of This Post)

                      10.  Part or Assembly cannot be renamed in context (must be done by opening drawing or closing out and renaming in file explorer).

                      11.  BOMs cannot be filtered through programming; must be done manually (haven't looked to deep into this one yet).

                      12.  No Single Member Patterns (Another One that Drives me Crazy)

                      13.  Mates don't disappear when the Part is deleted from the Assembly (I think).

                      14.  Sheet Metal features become unstable when part is rolled back and modified..

                      15.  External Reference Management:

                           a.  External References and Equations don't seem to hold up between configurations.

                           b.  Copying Assemblies sometimes breaks external references between assembly components.

                      16.  Equations cannot evaluate to 0 (this thread).

                       

                      Some of these cons could just be my inexperience with the software, so right now I'm a little biased .

                      Bob

                        • Re: Component Equation Won't Evaluate to 0?
                          Bernie Daraz

                          Thank you for your detailed response! I copied it out so I could delve into your thoughts in more detail. It's likely I won't comment further.

                          • Re: Component Equation Won't Evaluate to 0?
                            Dan Pihlaja

                            1.  Cannot Copy and Paste Mitre Flanges

                                    No idea here....

                            2.  Cannot do Sheet Metal Surface Rips

                                    I think that you might be able to, but I am not sure as I don't use sheet metal very often.

                            3.  No Auto Sketch Relations in Sketch Mode (Except Vertical and Horizontal)

                                    You are correct, however, check out these links:

                                          How to Quickly Fully Define Your SolidWorks Sketch | CATI Tech Notes

                                          What is Fully Defined sketch         

                            4.  The Drawing Does Not Copy when you Copy the Part or Assembly

                                    Again, correct.

                            5.  No Complex Cuts in Sheet Metal

                                     See # 2.

                            6.  Suppressing a Part Driven by an Assembly Equation Blows Up the Model (This one was really frustrating)

                                    Not sure about this one.

                            7.  String Variables cannot be created (Useful for bulk assigning Materials and Gauges).

                                     Don't know exactly what you mean by this

                            8.  Sheet Metal Conversions Are Not as Robust

                                     I will have to take your word for that one.

                            9.  Negative Dimensions Cannot Be Entered and Dimension Vector is Inconsistent (Part of This Post)

                                       I agree

                            10.  Part or Assembly cannot be renamed in context (must be done by opening drawing or closing out and renaming in file explorer).

                                      I think that this can be done in SW 2016.  See this link: 2016 SOLIDWORKS Help - Changing Component File Names from the FeatureManager Design Tree

                            11.  BOMs cannot be filtered through programming; must be done manually (haven't looked to deep into this one yet).

                                      With the right setup on parts/assemblies, this is easy.  After I have my assembly set up correctly (which is pretty fast with property tab builder and templates), all I have to do is drop the BOM into the drawing and it is how I want it......no rebuilding at all.   3 clicks.  Done.

                            12.  No Single Member Patterns (Another One that Drives me Crazy)

                                      Not really sure why you would want this, but you can copy and mirror which are kind of like this (I think)

                            13.  Mates don't disappear when the Part is deleted from the Assembly (I think).

                                      If you have this option ON they will:

                            Or click the "advanced" button to get this:

                               

                             

                            14.  Sheet Metal features become unstable when part is rolled back and modified..

                                      Sometimes true, I think this has more to do with workflow though

                            15.  External Reference Management:

                                a.  External References and Equations don't seem to hold up between configurations.

                                    See # 14

                                b.  Copying Assemblies sometimes breaks external references between assembly components.

                                      See # 14

                            16.  Equations cannot evaluate to 0 (this thread).

                                      True, but they CAN evaluate to .000001"  Which is close enough for most people.

                             

                            This wasn't meant as a dig.....I just saw some things that I could answer.  

                              • Re: Component Equation Won't Evaluate to 0?
                                Robert Millot

                                That's great info...thanks for your responses!  I'm definitely going to look into #3, #11, and #13.

                                 

                                For #1...in Pro/E you can Ctrl-C any feature in the model tree, then Ctrl-V and paste the feature on to the model by re-selecting references.  This is exceptionally useful for mitre flanges that have complex sketches.

                                For #6...If I type an equation into an assembly that drives the dimensions of a part, then I suppress the part, I get an error in the equation bank.  You get errors in the Pro/E equation bank as well, but it doesn't transfer to the model and you can keep working with a stable model.

                                For #7...in Pro/E you can create string variables in the Equations editor (i.e. MTL="304SS").  This is useful for exporting text into your documents for releasing your work to the floor.

                                For #12...When you use an equation to drive the pattern number, you sometimes end up with a value of 1 (which is acceptable in most of my applications).  Pro/E allows you to have a pattern with 1 element, Solidworks does not.

                                 

                                Bob

                              • Re: Component Equation Won't Evaluate to 0?
                                Jeremy Feist

                                #3: in addition to horizontal and vertical, I get coincident, midpoint, and tangent (and probably others that I am forgetting) added automatically.

                                Capture.PNG

                          • Re: Component Equation Won't Evaluate to 0?
                            Jeremy Feist

                            this may be a case of SW giving you the wrong error message. make sure that when that dim is 0, that it does not make an invalid sketch entity (such as a line of 0 length).

                            • Re: Component Equation Won't Evaluate to 0?
                              Steven Barry

                              Robert, any chance you could upload an example part?  Or perhaps give us what exact equation you are using?  Perhaps you are inadvertently dividing by zero somewhere?

                               

                              Also, is it evaluating EXACTLY to zero, or is there a chance there could be some trailing decimal places (e.g. 0.00000001)?

                               

                              If it's just a global variable that is set to equal zero, I don't see why you would experience this error.

                                • Re: Component Equation Won't Evaluate to 0?
                                  Robert Millot

                                  Steven,

                                   

                                  It is not a global variable...I can set global variables to zero with no problem.  It is an equation-driven dimension in the "Equations--Components" section that will be reduced to zero to control the pitch height of an angled sheet metal surface (see my photo in the OP).  Here is the equation:

                                   

                                  "PITCH_LEFT@Base@DT_SC<2>.Part"="PITCH_LEFT@Base"

                                   

                                  The equation simply drives the pitch height of the part from a sketch of the pitch height in the assembly.  There is no division by 0 or trailing zeroes, because the user directly enters the right side of the equation from the assembly.

                                  I have since found a workaround by re-dimensioning the part's pitch height from a different baseline, then  using subtraction in the assembly equation to arrive at the right dimension:

                                   

                                  "PITCH_LEFT@Base@DT_SC<2>.Part"="RR_HT@Base@DT_SC<2>.Part" - "PITCH_LEFT@Base"

                                   

                                  This works fine; it's just a shame that you can't set a dimension equal to zero using equations without getting that modeler resolution error.  It would make things much simpler.

                                   

                                  Bob