tapered threaded holes

[swhits]

I am trying to make a tapered threaded hole in a hydraulic manifold and the pipe threads do not show up as a tapered threaded hole. Is this feature possible in Solid Edge?

 

[swertel]

Yes, but not as easy at it should be.

There is a text file called pipethreads.txt. This has the information needed to generate the correct depiction of a pipe thread. Depending on whether this is an internal or external thread, you have to use protrusion or cutout with the exact values listed in pipethreads.txt. Once that feature is made, you use the thread feature to add your cosmetic thread.

I wish internal NPT and other pipethreads were available through the hole command, but they're not. Maybe in a future version.

--Scott

For some pleasure reading, try FAQ731-376

 

[fredericmenage]

Hi,

The method is to create a simple hole or cylindrical cutout. and then use the 'thread' command.

SE checks the diameter value of your hole against numbers in pipethreads.txt in the column 'inside pipe diameter' and allows you to apply that thread. The hole should then be represented as a tapered threaded hole in the draft views.


general behaviour: if it's a threaded shaft (protrusion), the diameter of that feature has to match one or several numbers in the 1st column in Pipethreads.txt and/or holes.txt; if it's a threaded hole, the diameter of that feature has to match one or several numbers in the columns 'inside pipe diameter' or 'internal minor diameter' in pipethreads.txt and/or holes.txt

HTH

Fred

 

[fwc]

Hi

FYI, if you couldn't find the threads you're looking for in that file you can always add new threads to it.


To simplify things, you may want to store these features (mainly consists of a cutout/protrusion and the thread) in feature library for future use. The next time you create the thread, it is only drag and drop it into the part environment.


Regards

fwc