4 Replies Latest reply on Oct 3, 2014 1:52 PM by David Urasky

    Internal Thread

    Akshay Patel

      Hello friends,

      I got a component to design in solidworks in my job, but I am stuck at point so need your help. Here I am attaching Solidworks file. In top surface there are two holes in which I need an internal threading. i tried  swept cut but didn't work. So please can anybody suggest me how to approach.?

      Also I highlighted in image.

        • Re: Internal Thread
          Ian Worrall

          Create these holes using the "Hole Wizard" feature, set to add a "Cosmetic Thread" to the holes.

           

          HoleWiz.PNG

          • Re: Internal Thread
            Lenny Bucholz

            SW doesn't model the 3d thread ituses hole wizard it puts in the correct drill size for the tapped hole desired and puts a bit mapped pic in the hole to represent the thread.

             

            if you need to have 3d threads you must model them using the correct dims as in the machinery handbook.

            • Re: Internal Thread
              Theo Linders

              In the holewizard you can apply a cosmetic thread.

              When you want to see a real thread you have to model it yourself by first making a hole at drillsize and then, using cut sweep combined with helix, to cut this thread into your part.

              What is the reason you need to see the threads? There is no real mechanical reason for this.

               

              good luck

              Theo

              • Re: Internal Thread
                David Urasky

                Akshay,

                 

                It sounds like you need to accurately depict cut threads in the holes. So here's how you do it;

                 

                • I used your part to make them beginning with helix 1 which you created using the circle on the top of the hole. I made one modification to the helix settings, I changed the start angle to 0 so I can do the next step easily.

                10-3-2014 11-22-13 AM.png

                • I created a plane parallel to the right plane at the endpoint of the helix. Now the plane is 90 degrees to the axis of the helix.
                • Start a sketch on the new plane and look normal to it. Create the shape which depicts the actual thread form. I created an SAE 60 degree thread form. This information can be found online or the Machinery's Handbook. The width of the thread cannot be => the pitch of the helix so I arbitrarily subtracted .005" from the pitch. If the width of the thread matches the pitch there will be a zero thickness error. I also made the corner of the triangle coincident with the end of the helix.

                10-3-2014 11-35-32 AM.png

                • Then use this sketch as the profile in a swept cut. The helix will be the path.

                 

                If you want to make this realistic, you have some problems. The hole size seems strange, .26". This hole size is for what thread? The pitch of the helix is .03", this gives thread of 33.33 threads per inch (TPI).

                 

                If you are simulating an actual thread, use the hole wizard to create a threaded hole to the desired configuration. When you do this do not display any threads. Now the hole size is correct for that thread and you know the TPI. Next create your helix with the pitch of the 1/TPI and the desired depth. Use the height & pitch option to do this.

                 

                Then using some resource determine the actual shape and size of the thread form to create the sketch used for the profile.

                 

                Then cut the threads.

                 

                I was going to attach the part file, but I see you are using an older version of SWX. So it would do no good. so a picture of the section.

                10-3-2014 11-51-14 AM.png