9 Replies Latest reply on Jun 4, 2015 12:08 PM by Asdfa Afsdaff

    Create engraved labels to put on machinery.

    David Clabough

      We have been adding more and more labels to our machinery, to the point the labels are now being treated as fabricated parts. We were creating a single part, and setting up a design table to alter size and text for the label, and extrude-cut the text. This showed up well in the assembly, and we could make drawings for fabricating the labels. We discovered that our fab shops were having to re-create the text because their machine requires a "stick" font to create a single line path for the engraving tool. This is not acceptable due to typos and redoing work that was already done. We have changed the label so that it is just a sketch and not extrude-cut. This works OK, and keeps part file simpler for rebuilds. We have two problems with this method though. First the drawing for the labels requires us to do a "Reset Sketch Visibility" for each view, to ensure we have the latest info in the label. There is not a global command to reset all the views, which could be quite a few depending on the machine. Second, in the assembly file and assembly drawing, the sketch shows up in all views, or none. The assembly drawing views are really the most important. If looking at the left side of an electrical cabinet, the sketches show up for the labels and look correct, but in the right view, they "bleed" through to the other side. I can toggle the "View Sketches" and it removes all the sketches, and the label text no longer shows up. I can individually "hide" the sketches for each label in each view, but again this is not practical due to the number of labels and drawing views.


      What are other people doing for machine labels and drawings for them?




        • Re: Create engraved labels to put on machinery.
          Asdfa Afsdaff

          Have you tried using a wrap instead of a sketch or extrude-cut?

            • Re: Create engraved labels to put on machinery.
              David Clabough

              I just tested it, and it works like the extrude-cut but for curved surfaces. What I am understanding for engraving on CNC equipment, is they need a centerline tool path to program to. When they get an extrude-cut, it is a closed contour, with no real centerline. With any of the extrude-cuts, the CNC would look at text as though it were a series of very small pockets to mill out, but for engraving they just need a single line for an engraving tool to follow. I have to believe other people are putting labeling, etc. in their models and I am curious as to what they are doing.


              Thanks for the help.

            • Re: Create engraved labels to put on machinery.
              Jim Sculley



              SW 2015 added a stick font capability.


              Unfortunately, it doesn't solve your other problems.  If you search the forums for silkscreen you'll find plenty of other discussions on this topic with no really viable solutions.


              Jim S.

              • Re: Create engraved labels to put on machinery.
                Chris Mackedanz

                I have the same issues!


                Our engraving department can import dxf's.  The problem comes in that to get the text to show up correctly you have to use sketch text, and extrude cuts to make it look correct.  When our engraving guy gets the dxf he see's the outline of the text...which his engraver then follows.  This takes longer than it should.


                So he has to remove the lines that came in for the text, and add it back in as text in his engraving software, so he has single line "stick" font that works well in the engraver.


                I've tried creating the engraving in Draftsight as a sketch (there are some decent "stick" type fonts in there) and then bringing that in and putting it on the engraving part... but then I run into all of the problems about showing/hiding sketches and their visibility.


                What seems to work out ... ok ... is to have two configurations in the part, the default one would just be the overall size of the engraving, and it's thickness... your engraving without any text.  Put all of the extrude-cuts in / on another configuration, so you CAN show them for rendering and to wow the clients.  Then when you go to make the drawings (and dxfs from them ) you use the default config to get the overall size of the engraving, and then use a standard solidworks annotation to put in the text.  When it's exported the text is imported (at least in ours) as text.  It may not be the right font, and your engraving guy will have to tweak it a little bit to get it to be right again but it's a lot better than them having to retype everything ... and maybe get things wrong...


                There is no good way of doing it that i've found ...

                  • Re: Create engraved labels to put on machinery.
                    David Clabough

                    Thanks for tips. The alternate configuration is a good idea, and I may try that. The biggest problem I see with that in my case, is that I use a single part and create multiple configurations through a design table. This table may create 30 different labels. We have run into situations where the rebuild of the configurations can take a while and crash sometimes, when using extrude-cut. I would really like to just use the sketch only, because it is much easier on the rebuild time.


                    I put in a request for an enhancement (ER number 1-8159772858) to make this a built in function that will work easily in all situations. If you have time you might go and "like it" or whatever it offers to maybe get SW to look into it. I have never put in a request, but felt this might be something others could use. It seems like it should be much simpler than it is turning out to be.

                  • Re: Create engraved labels to put on machinery.
                    Erik Lund

                    Here you go...


                    OneLineFonts, The source for single line fonts


                    Unfortunately, SW isn't the best for generating tags.  I prefer to use Draftsight for that.  If you do want to generate your tags/labels in SW I suggest using the 'scribe' command and NOT extrude/cut.

                    • Re: Create engraved labels to put on machinery.
                      Jamil Snead

                      Instead of toggling sketch visibility on the drawing another option is to leave sketches hidden in all views, and in the views where you want the text shown you can select the sketch form the tree and convert entities onto the drawing. I think you may need to convert the text to sketch entities for this to work.  I don't know how well this behaves if the sketch is altered, like I am not sure if new text added will automatically get converted onto the drawing. Maybe that is work experimenting with.