10 Replies Latest reply on Jul 2, 2014 5:59 PM by Scott Rypstra

    Threaded holes on Drawings

    Wayne Schafer

      I used the hole wizard in assembly features to but a 10-32 threaded hole in an assembly.  But when I go to the detail the assembly the hole does not show as a thread hole but when I use the hole callout it calls it out a thread hole.  What do I need to turn on to make it look like a threaded hole on the detail drawing?  I am using SW 2012 SP2.

        • Re: Threaded holes on Drawings
          Matt Neuman

          In the drawing, go to Insert, model items.  Then, under Source, select "Entire Model", under dimensions, click off the dimension icon and under annotations, click on the cosmeticthread.  Also, make sure the "Import items into all views" box is checked.  I believe you only have to do this with assemblies, parts always bring in the cosmetic threads, not sure why assmeblies don't.

           

          Capture.PNG

           

            • Re: Threaded holes on Drawings
              Sumit Pokhrel

              I have exactly done this to no vail  . I want to create a #6-32 hole on a square steel plate. It just creates holes but no threads

                • Re: Threaded holes on Drawings
                  Lenny Bucholz

                  Never has made threads with the hole wizard. Yes there a cosmetic image but again it's not threads either.

                   

                  if you need to have threads you need to model all the hole with a cut sweep.

                   

                  or go to mcmaster.com downloae the size screw your using bring a part in a part and use the combine tool to subtract the bolt \screw from the hole.

                   

                  drafting\detailing standards don't show the threads either, notes and hidden lines are the norm, for prodution, machinist don't need to see the threads to know what to put in a part.

                   

                  only time really need is for brochures and pretty pics for sales, not manufacturing.

                    • Re: Threaded holes on Drawings
                      Sumit Pokhrel

                      Thanks Lenny. That Helps. Can you elaborate more on "using the combine tool to subtract the bolt \screw from the hole" ? I will be very grateful .

                        • Re: Threaded holes on Drawings
                          Lenny Bucholz

                          here is a link for explaining:

                          http://compgroups.net/comp.cad.solidworks/combine-subtract-diffrence/19155

                           

                          help file:

                           

                          Combine Bodies

                          You can combine multiple solid bodies to create a singled-bodied part or another multibody part.

                          It is strongly recommended that you do not use the Combine feature to combine weldment bodies. It is not always possible to calculate the cut list properties accurately for a body created using the combine feature.

                          There are three ways to combine multiple solid bodies:

                          •   Add. Combines solids of all selected bodies to create a single body.

                          •   Subtract. Removes overlapping material from a selected main body.

                          •   Common. Removes all material except that which overlaps.

                          To use the Add or Common operation type:

                          1.   Click Combine on the Features toolbar, or click Insert, Features, Combine

                            The Combine1 PropertyManager appears.

                          2. Under Operation Type, click Add or Common.

                          3. Under Bodies to Combine, select the bodies in the graphics area, or select the bodies from the Solid Bodies folder in the FeatureManager design tree.

                          4. Click Show Preview to preview the feature.

                          5. Click OK .

                          To use the Subtraction operation type:

                          1.   Click Combine on the Features toolbar, or click Insert, Features, Combine

                            The Combine1 PropertyManager appears.

                          2. Under Operation Type, click Subtract.

                          3. Under Main Body, select the body to keep from the graphics area for Solid Body , or select the body from the Solid Bodies folder in the FeatureManager design tree.

                          4. Under Bodies to Subtract, select the bodies whose material you want to remove for Solid Bodies .

                          5. Click Show Preview to preview the feature.

                          6. Click OK .

                  • Re: Threaded holes on Drawings
                    Mike Agan

                    Also is the center box on in attached?Capture.PNG

                    • Re: Threaded holes on Drawings
                      Adam Benson

                      You will also want to make sure you are displaying the 'shaded cosmetic threads'. Right click on the annotations folder, select details, and check shaded cosmetic threads.

                       

                      Hope this helps

                      • Re: Threaded holes on Drawings
                        Robert Berry

                        Good luck Wayne

                         

                        I've had horrible luck with cosmetic threads.

                         

                        The hidden line root dia only shows up on the side of the sketch plane created with the hole wizard, in the model and the detail.

                         

                        I sometimes get representation of all the tapped holes in an assy, (in all the views),  and the only way to get rid of them is to hide them.

                         

                        The root hidden lines don't show up in the angled side of aligned sections.

                         

                        I've sent the offending files to the VAR and they have sent them to Solidworks and I get the age old reply, there is an SPR for that and it's a known bug,thanks for reporting it, Blah blah blah

                         

                        I'm still using 2010, maybe it will be better in 2012, but I have no confidence that it will change judging from the response from Solidworks.

                         

                        Again best of luck

                         

                        I've set all of my setting to those suggested above to no avail.

                        • Re: Threaded holes on Drawings
                          Scott Rypstra

                          WOW I finally found this: find the feature in the tree under the view you want the thread to show; right-click the feature->Show/Hide->Show Hidden Edges.

                          Note, I have SW 2012 SP 5.0