Having a problem threadmilling NPT in X9

[Sticky]

I'm having some difficulty getting thread milling working correctly in mcfswx9.

 

I do have one set of files in mcfsw X9 that are working correctly, which are using pre X9 tapered tool definitions, or custom tool definitions.

 

Now I am trying to use the new tool manager thread mill option. IIRC the old way you used the minor diameter of the cutting tool for the cutting diameter. In X9 it looks like you use the shank diameter?

 

This is for a 1/8 npt threadmill, this is how it would have been defined pre X9 if it were a taper mill. The image preview does not look like the tool in real life.

 

And if I change the "outside diameter" to the shank diameter, then the image preview looks correct.

 

Regardless of how it is defined, the cutter never gets close to the wall of the hole, so it doesn't cut any threads.

 

I am using a .339" diameter circle to drive the threadmill toolpath. Here are the parameters for the threadmill toolpath.

 

 

I can't figure out what I am doing wrong. I've worked a few 16hr days in a row this last week though, hopefully it's just something simple. I'll be back tomorrow to try this again.

 

 

[crazy^millman]

Have you tired to use the old school helix method. Draw the helix and drive it with 3D Contour how we did it before all the new stuff. Cut many threads that way and still do when Mastercam does this weird stuff and I need to get the job done after one of those 16 hour days. Best of luck getting it figured out.

 

To me everything looks correct.

[gcode]

I've always defined NPT treadmills as the minor diameter

Offhand I don't know the driving diameter for an 1/8" NPT,

but Carmex has an excellent thread milling calculator  you can

download

 

http://212.235.101.236/

 

this is the first place I go for troublesome treadmill situations

[Sticky]

Have you tired to use the old school helix method. Draw the helix and drive it with 3D Contour how we did it before all the new stuff. Cut many threads that way and still do when Mastercam does this weird stuff and I need to get the job done after one of those 16 hour days. Best of luck getting it figured out.

 

To me everything looks correct.

 

No I haven't done the helix yet. I certainly could, but as I was working on this group of parts I decided I was just going to make a file full of npt threadmill ops so that I could build a whole library full of them to make running waterlines and such more automated.

 

This is the first time I've played with the tool manager's threadmill definition.

 

I've always defined NPT treadmills as the minor diameter

Offhand I don't know the driving diameter for an 1/8" NPT,

but Carmex has an excellent thread milling calculator  you can

download

 

http://212.235.101.236/

 

this is the first place I go for troublesome treadmill situations

 

The weird thing is that is it doesn't matter what diameter I use, it still won't cut to the edges to the hole. You can make the diameter large enough that it can't make a toolpath, and everything below that point stays away from the edge of the hole.

 

I wonder if there is some sort of issue between the arc and the point selection in mcfsw?

 

Is anyone successfully using the npt threadmilling in mcfsw X9?

[gerrythewelshman]

Hi,

    I am new to the X9 but this is what I do.

1. get to : select a tool 

2. right click select 'create a new tool'

3.Thread mill

4. thread type      NPT

5. now you have more info than what you had in your window

6. at the base see thread angle  

 

hope this helps

 

GTW     (gerrythewelshman)

[gcode]

^{According to the Carmex data your driving diameter should be .403"}

 

^{this is the program Carmex yields}

^{they are defining the tool diameter as .230"}

^{note the thread mill code is G91}

^{there is no option to post out G90 code so its hard to compare}

^{Carmex output to MC output}

 

^{%
O151
( FANUC I&J, RH, CLIMB, INTERNAL THREAD MILLING )
( TOOL - MT0250C03 27NPT )
( THREAD - 27 TPI, DIAMETER 0.403 INCH, DEPTH 0.264 INCH )
( TOOL RADIUS COMPENSATION  D1=0 )
N1 T1 M06
G90 G00 G54 G40 G17 G94 X0.0000 Y0.0000 S7900 M03
G43 H1 Z1.9685 M08
( PASS NUMBER - 1 )
G90 G01 Z-0.2686 F196.9
G91 G01 G41 D1 X0.0452 Y-0.0452 F4.9
G03 X0.0452 Y0.0452 Z0.0046 I0.0000 J0.0452
G03 X-0.0904 Y0.0907 Z0.0093 I-0.0907 J0.0000 F14.8
G03 X-0.0910 Y-0.0907 Z0.0093 I0.0000 J-0.0910
G03 X0.0910 Y-0.0913 Z0.0093 I0.0913 J0.0000
G03 X0.0916 Y0.0913 Z0.0093 I0.0000 J0.0916
G03 X-0.0458 Y0.0458 Z0.0046 I-0.0458 J0.0000
G01 G40 X-0.0458 Y-0.0458 F196.9
G90 G00 Z1.9685
M30
%}

[Sticky]

Hi,

    I am new to the X9 but this is what I do.

1. get to : select a tool 

2. right click select 'create a new tool'

3.Thread mill

4. thread type      NPT

5. now you have more info than what you had in your window

6. at the base see thread angle  

 

hope this helps

 

GTW     (gerrythewelshman)

 

Gerry, is there any chance you could take a screen shot of that? I'm not getting the additional options as you suggest. It could be that mcfsw doesn't have that option?

 

^{According to the Carmex data your driving diameter should be .403"}

 

^{this is the program Carmex yields}

^{they are defining the tool diameter as .230"}

^{note the thread mill code is G91}

^{there is no option to post out G90 code so its hard to compare}

^{Carmex output to MC output}

 

 

 

I'd rather not make make my tool diameter smaller than it is in real life, this causes problems with production and operators. Any chance you could try making a threadmill in X9 and mcfsw X9 and see if you get the options that Gerry is getting above? I don't have standalone X9 on my computer.

[gerrythewelshman]

see capture

 

 

 

 you must put in correct info and angle  

[gerrythewelshman]

 

 

as soon as you get to select tool  RIGHT CLICK  and select thread mill tool

[Sticky]

Interesting. I was not using right click. I'm already gone for the day but I will try that first thing tomorrow morning. Thank you.

[gcode]

you don't make the tool smaller than real life

define it as it's true tip diameter and drive the tool path  with a .403" circle

and set your depth to -.264

the thread will come out a couple of thousands small allowing for CDC for final adjustments

I've been using  a straight end mill definition for years to cut NPT

I did some tests this morning

first tool path used an end mill @ .230" dia

the 2nd used the new threadmill @.230 dia

 

the posted code was identical

the threads and  taper in the new thread mill are eye candy... the .230" value drives the posted code

[civiceg]

I noticed your diameter is grayed out the 1.0". I have had an issue when selecting on a solid, it picks whatever diameter is on the solid and it can't be changed.... grayed out. So I would create a point on another level, turn off the solid level and drive off a point, allowing you to adjust the diameter to your liking. 

 

I have gotten bit by selecting directly off a solid once, never again. 

[gcode]

I draw a circle with the correct diameter and chain that

[civiceg]

I like seeing the actual diameter in the input, but that works too. 

[gcode]

I filed a bug report for this

when chaining a circle in circle tool path we should see the grayed out diameter of the circle,

not a grayed out 1

I was told it will be fixed in MC2017

[civiceg]

I am pretty sure if you create your own circle in older versions X6ish it would not be grayed out, but in X9 it is like you said. I stopped using a circle around x6 so I never noticed until now. 

[crazy^millman]

Why I have used point for many years to avoid this very issue. Caries over to many methods and process from this to 5 Axis. Yes we have had many conversations about this, but end of the day when you need to get the job done lost the extra hassle is just not worth it.

[Sticky]

Capture.PNG

 

 

as soon as you get to select tool  RIGHT CLICK  and select thread mill tool

 

That is for the shank only from what I can tell, it has no effect on the cutting geometry.

 

you don't make the tool smaller than real life

define it as it's true tip diameter and drive the tool path  with a .403" circle

and set your depth to -.264

the thread will come out a couple of thousands small allowing for CDC for final adjustments

I've been using  a straight end mill definition for years to cut NPT

I did some tests this morning

first tool path used an end mill @ .230" dia

the 2nd used the new threadmill @.230 dia

 

the posted code was identical

the threads and  taper in the new thread mill are eye candy... the .230" value drives the posted code

 

The small end if my Morse 1/8 NPT threadmill is .278". I would assume that .23" is the small end of the carmex threadmills?

 

Edit* I just looked up some Carmex threadmills and their standard 1/8npt threadmills have the small diameter listed as .250" for solid, and .299" for TSC. Their 1/16npt does have a .23" small end though.

[gcode]

Yes.. enter to small end of the tapered thread mill into the cutting diameter of the tool definition

The interactive Carmex app gave me 2 solid carbide thread mills for 1/8-27 NPT

 

see the attached screen shot

 

If you drive a Ø.403 circle" at a depth of .264 and define the tool as described above,

you will get a good thread

CARMEX NPT.pdf

[gerrythewelshman]

see capture

 

Capture.PNG

 

 

 you must put in correct info and angle  

This was just a photo and has no correct info in it .

I to always used the same system as gcode but came across this way.

It does the same thread

[hydranamics]

Are you using the threadmill toolpath? I currently use a drawn toolpath and 2D contour. However I experienced the same issue with the threadmill defined tool where the tool is offset from my toolpath. to correct this when creating a new tool I define the outside tool diameter as the actual tools outside diameter, then in the 2D contour toolpath Cut parameters I just put (1/2 the difference between the tools large diameter and small diameter) in the Stock to leave on walls field as a negative number.