Applying a knurl detail
Applying a knurl detail
(OP)
I am trying to apply a knurling to a round bar, and am having trouble coming up with the best way to do this. Has anybody done this before or know what the best way to do this would be?
Thanks in advance,
Lurks
Thanks in advance,
Lurks





RE: Applying a knurl detail
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Applying a knurl detail
2.) I am running NX5.
Thanks,
Lurks
RE: Applying a knurl detail
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Applying a knurl detail
RE: Applying a knurl detail
No prizes for guessing what it is, but as a hint check the website
BTW NX-5 Okay?
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
RE: Applying a knurl detail
Note that the model is fully parametric in that if you edit the 'Shaft_Diameter' or the 'Shaft_Length', the model will update. However, you will note that the model is not fully finished as the final subtract operation has not yet been performed, for two reasons. First, in order to be fully parametric you need to edit the parameters BEFORE performing the Boolean subtract since depending on the diameter of the shaft entered there will be a different number of tool solids for that final Boolean operation. Also note that if you do edit the 'Shaft_Diameter' that it must a fractional number which is a multiple of 1/64 inch.
The second reason is that the part file, before the Boolean operation, is an order of magnitude smaller than after.
So to get your finished model, first edit the expressions 'Shaft_Diameter' and/or 'Shaft_Length', entering your desired size(s), and hit OK, and after the model updates perform a Boolean Subtract selecting the shaft as the Target Body and then do a 'select-all' (or drag-select the screen) to select ALL of the Tool Bodies and hit OK (it will take a while before this operation is completed).
Below is a image of a completed Knurled Knob:
Now note that there are actually 4 different Knurling sizes, 64, 96, 128 and 160 Diametral Pitch and so if you need one of the other sizes, you can refer to the standard referenced above noting that in addition to the Expression for the Diametral Pitch, you will also need to change the value for the Tooth Depth and something called the 'Tracking Factor' (all of these names are referenced in the 'Comment' column of Expression dialog).
As a help, if you have a Machinery' Handbook (25th edition) you can find a table of these values starting on page 1148. Note that the names of all of the relevant Expressions are consistent with the names shown in the standard so that should make it easy for you to find what you need if there's ever a need to make any changes.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Applying a knurl detail
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
RE: Applying a knurl detail
I don't know about how you guys do it in 'OZ', but here in the 'civilized' world, diagonal knurling is angled at 30 degrees to the axis of the shaft, not 45
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Applying a knurl detail
Best Regards
Hudson
www.jamb.com.au
Nil Desperandum illegitimi non carborundum
RE: Applying a knurl detail
Lurks
RE: Applying a knurl detail
RE: Applying a knurl detail
This brings up a related question: occasionally when performing boolean operations I will get this error. Things that I'm sure would have united or subtracted in NX2 simply won't work in NX6. It is difficult to reproduce this error, but if it pops up in a file that I can post, I will.
RE: Applying a knurl detail
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.
RE: Applying a knurl detail
So attached is slightly modified model where I've made i easy to first select the tool bodies which create one set of diagonals and the second set for the other.
So after opening the part file, do a Boolean subtract, selecting the central core as the target body and the 64 other bodies as the tool bodies all in one operation. After that completes, do a Show all hidden bodies and repeat the above step, and you will have to your finished model.
John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Cypress, CA
http://www.siemens.com/plm
http://www.plmworld.org/museum/
To an Engineer, the glass is twice as big as it needs to be.