Applying a knurl detail 2

[lurks]

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

 

[JohnRBaker]

Is this for visual purposes only, such as for a photo-realistic rendered image, or do you actually need a 3D physical model of the knurling? Also what version of NX are you running?

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.

 

[lurks]

1.) I need an actual 3D model of the knurling.
2.) I am running NX5.

Thanks,

Lurks

 

[JohnRBaker]

Do you want straight knurling or diagonal? And if Diagonal, single or double? Note that the only 'standard' I can find for knurling is for Imperial Units (inches).

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.

 

[lurks]

These parts have a double diagonal knurl. Imperial units is exactly what I'm looking for.

 

[hudson888]

There you go attached is an example of a knurled model. Perhaps not the best or only way to hit it but for what I needed, serviceable!

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

 

[JohnRBaker]

OK, attached is a part file representing a 1 inch Nominal Diameter 'Knurled' knob, 1/2 inch wide. It's has a double-diagonal 64 Diametral Pitch Knurling based on the the ANSI/ASME B94.6-1984 standards.

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.

 

[hudson888]

Darned upload never works for me! the file is attached here

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

Hudson,

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.

 

[hudson888]

Artistic License it was only for looks anyway!

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[lurks]

Thank you both for the helpful tips. That is exactly what I'm looking for.

Lurks

 

[BOPdesigner]

John, What is the trick to get the boolean operation you describe to work in NX 6 (6.0.2.8). I get an "unable to perform boolean error" or if I increase the tolerance value on the subtract settings, I get a Thru face does not intersect path of the tool.

 

[cowski]

I'm also running NX6.0.2.8 and I get the same error.

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.

 

[JohnRBaker]

I'll check it out.

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.

 

[JohnRBaker]

OK, we did a little 'research' and came up with a solution to the problem. Due to some changes made in NX 6.0 where, irrespective to the number of tool bodies selected, only a single Boolean feature is created (in NX 5.0 you get 1 feature for each tool body selected). However, there are some issues with respect to the number of tool bodies, particularly if they 'interfere' with each other. However we learned that rather than selecting all 128 tool bodies in one operation, we were to select only half, 64 in Boolean subtract operation and after it completes, select the second set of 64 tool bodies, while this does result in 2 Boolean features instead of one, it's still much better than 128 which was the case in NX 5.0.

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.