Threadmilling - X9

[Mick]

Programming an ID  threadmill operation in X9, and using multi passes.

 

I choose the centre of the arc representing the OD of the thread.  The thread height (as a radius) is 1.484mm

 

Setting the Multi pass depth of cut to .433mm @ 3 passes and then 1 finish pass at .1mm, should work out at close to three even roughing cuts and then one finishing cut. However, when I generate the toolpath, the first pass is at approximately half depth.

 

To achieve the even roughing passes, I had to set it to 6 roughing passes. It is almost like it seems to be a diameter setting for the stepover of passes?

 

If that is the case, I wasn't aware of that.

 

 

[Guest]

I do threadmilling a bit different than you do.....I select the arc....

 

I created a .500 diameter arc, used a .250 dia tool and set 2 cuts at .02 and a finish at .005

 

N112 G0 G90 G54 X0. Y0. S1000 M3

N114 G43 H1 Z.25

N116 Z.1

N118 G1 Z-.25 F25.

N120 X.0389 F5.

N122 G41 D1 X0. Y-.0625

N124 G3 X.0389 Y-.0736 I.0389 J.0625

N126 X.1125 Y0. I0. J.0736

N128 Z-.2 I-.1125 J0. <--------------

N130 X.0389 Y.0736 I-.0736 J0.

N132 X0. Y.0625 I0. J-.0736

N134 G1 G40 X.0389 Y0.

N136 X0.

N138 Z-.25 F25.

N140 X.0398 F5.

N142 G41 D1 X0. Y-.0725

N144 G3 X.0398 Y-.0827 I.0398 J.0725

N146 X.1225 Y0. I0. J.0827

N148 Z-.2 I-.1225 J0.<-------------------

N150 X.0398 Y.0827 I-.0827 J0.

N152 X0. Y.0725 I0. J-.0827

N154 G1 G40 X.0398 Y0.

N156 X0.

N158 Z-.25 F25.

N160 X.04 F5.

N162 G41 D1 X0. Y-.075

N164 G3 X.04 Y-.085 I.04 J.075

N166 X.125 Y0. I0. J.085

N168 Z-.2 I-.125 J0.<------------------

N170 X.04 Y.085 I-.085 J0.

N172 X0. Y.075 I0. J-.085

N174 G1 G40 X.04 Y0.

N176 X0.

N178 G0 Z.1

N180 Z.25

N182 M11

N184 M5

N186 G91 G28 Z0.

N188 G28 X0. Y0.

N190 M30

 

All diameter cuts as I set them are output at the values I would expect to see.....

 

The I-.125 being final and leaving .005 for a finish cuts, that's .0025 per side so the last roughing pass would be at .1225

The I.1225 being the final rough pass and setting to 2 passes at .020 that's .010 per side so the .1125 pass would be correct

 

So your passes at .1125, .1225 and .125 are correct

 

When you use multiple roughing passes the very first path is a calculated distance from your finished number based on the ending diameter.

 

I'm not sure if I that explanation makes it better or worse

 

If you really want even cuts all the way in......subtract your minor from your major, divide it by 2(per side distance) then subtract your

desired finish cut amount and dived the remaining by how many cuts you want......that value would then be your step over....

 

Thread milling does not recognize the anything but the geometry size to be cut

[RsH01]

"If you really want even cuts all the way in......subtract your minor from your major, divide it by 2(per side distance) then subtract your
desired finish cut amount and dived the remaining by how many cuts you want......that value would then be your step over...."

 

And they say:

Mastercam Mill delivers fast, easy, industry-proven NC programming that lets you make the most of your machines. The Mill suite of CAD/CAM tools is focused on delivering speed and efficiency to your shop.

[Mick]

I do threadmilling a bit different than you do.....I select the arc....

 

I created a .500 diameter arc, used a .250 dia tool and set 2 cuts at .02 and a finish at .005

 

N112 G0 G90 G54 X0. Y0. S1000 M3

N114 G43 H1 Z.25

N116 Z.1

N118 G1 Z-.25 F25.

N120 X.0389 F5.

N122 G41 D1 X0. Y-.0625

N124 G3 X.0389 Y-.0736 I.0389 J.0625

N126 X.1125 Y0. I0. J.0736

N128 Z-.2 I-.1125 J0. <--------------

N130 X.0389 Y.0736 I-.0736 J0.

N132 X0. Y.0625 I0. J-.0736

N134 G1 G40 X.0389 Y0.

N136 X0.

N138 Z-.25 F25.

N140 X.0398 F5.

N142 G41 D1 X0. Y-.0725

N144 G3 X.0398 Y-.0827 I.0398 J.0725

N146 X.1225 Y0. I0. J.0827

N148 Z-.2 I-.1225 J0.<-------------------

N150 X.0398 Y.0827 I-.0827 J0.

N152 X0. Y.0725 I0. J-.0827

N154 G1 G40 X.0398 Y0.

N156 X0.

N158 Z-.25 F25.

N160 X.04 F5.

N162 G41 D1 X0. Y-.075

N164 G3 X.04 Y-.085 I.04 J.075

N166 X.125 Y0. I0. J.085

N168 Z-.2 I-.125 J0.<------------------

N170 X.04 Y.085 I-.085 J0.

N172 X0. Y.075 I0. J-.085

N174 G1 G40 X.04 Y0.

N176 X0.

N178 G0 Z.1

N180 Z.25

N182 M11

N184 M5

N186 G91 G28 Z0.

N188 G28 X0. Y0.

N190 M30

 

All diameter cuts as I set them are output at the values I would expect to see.....

 

The I-.125 being final and leaving .005 for a finish cuts, that's .0025 per side so the last roughing pass would be at .1225

The I.1225 being the final rough pass and setting to 2 passes at .020 that's .010 per side so the .1125 pass would be correct

 

So your passes at .1125, .1225 and .125 are correct

 

When you use multiple roughing passes the very first path is a calculated distance from your finished number based on the ending diameter.

 

I'm not sure if I that explanation makes it better or worse

 

If you really want even cuts all the way in......subtract your minor from your major, divide it by 2(per side distance) then subtract your

desired finish cut amount and dived the remaining by how many cuts you want......that value would then be your step over....

 

Thread milling does not recognize the anything but the geometry size to be cut

 

John,

 

Thanks for the reply. Yes, I know how it calculates the depths of cut. And by picking the centre of the arc, it recognises the major diameter of the thread (the same as actually picking the arc). I subtracted the minor diameter from the major diameter, divided by two, and then removed the finish pass allowance, and then divided by four (four roughing cuts). That should have output four evenly spaced roughing cuts from the root diameter. However, the first cut was approximately half depth of the thread, then it proceeded to cut the multi passes correctly, albeit in shallower cuts than expected. That tells me it calculates it on diameter. And your output confirms that. I just find it weird, as all other milling is a radius amount.

 

If the "Step Over for Roughness" is clicked it highlights the Stepover, but shows it radially, whereas the output is actually on diameter.

 

G1 G40 Y0.

Z-25.536 F1000.

G42 D19 Y6.508 F175.

G2 X-100.992 Y0. Z-26.114 I3.914 J-6.508

X-124.008 Z-27.269 I-11.508

X-100.992 Z-28.423 I11.508

X-112.5 Y-6.508 Z-29. I-7.594

G1 G40 Y0.

Z-2.445 F1000.

G42 D19 Y6.867 F175.

G2 X-100.633 Y0. Z-3.023 I3.947 J-6.867

X-124.367 Z-4.177 I-11.867

X-100.633 Z-5.332 I11.867

X-112.5 Y-6.867 Z-5.909 I-7.92

G1 G40 Y0.

[swanny]

I do threadmilling a bit different than you do.....I select the arc....

 

I created a .500 diameter arc, used a .250 dia tool and set 2 cuts at .02 and a finish at .005

 

N112 G0 G90 G54 X0. Y0. S1000 M3

N114 G43 H1 Z.25

N116 Z.1

N118 G1 Z-.25 F25.

N120 X.0389 F5.

N122 G41 D1 X0. Y-.0625

N124 G3 X.0389 Y-.0736 I.0389 J.0625

N126 X.1125 Y0. I0. J.0736

N128 Z-.2 I-.1125 J0. <--------------

N130 X.0389 Y.0736 I-.0736 J0.

N132 X0. Y.0625 I0. J-.0736

N134 G1 G40 X.0389 Y0.

N136 X0.

N138 Z-.25 F25.

N140 X.0398 F5.

N142 G41 D1 X0. Y-.0725

N144 G3 X.0398 Y-.0827 I.0398 J.0725

N146 X.1225 Y0. I0. J.0827

N148 Z-.2 I-.1225 J0.<-------------------

N150 X.0398 Y.0827 I-.0827 J0.

N152 X0. Y.0725 I0. J-.0827

N154 G1 G40 X.0398 Y0.

N156 X0.

N158 Z-.25 F25.

N160 X.04 F5.

N162 G41 D1 X0. Y-.075

N164 G3 X.04 Y-.085 I.04 J.075

N166 X.125 Y0. I0. J.085

N168 Z-.2 I-.125 J0.<------------------

N170 X.04 Y.085 I-.085 J0.

N172 X0. Y.075 I0. J-.085

N174 G1 G40 X.04 Y0.

N176 X0.

N178 G0 Z.1

N180 Z.25

N182 M11

N184 M5

N186 G91 G28 Z0.

N188 G28 X0. Y0.

N190 M30

 

All diameter cuts as I set them are output at the values I would expect to see.....

 

The I-.125 being final and leaving .005 for a finish cuts, that's .0025 per side so the last roughing pass would be at .1225

The I.1225 being the final rough pass and setting to 2 passes at .020 that's .010 per side so the .1125 pass would be correct

 

So your passes at .1125, .1225 and .125 are correct

 

When you use multiple roughing passes the very first path is a calculated distance from your finished number based on the ending diameter.

 

I'm not sure if I that explanation makes it better or worse

 

If you really want even cuts all the way in......subtract your minor from your major, divide it by 2(per side distance) then subtract your

desired finish cut amount and dived the remaining by how many cuts you want......that value would then be your step over....

 

Thread milling does not recognize the anything but the geometry size to be cut

Why isn't there a Z move on line N124?

[Guest]

Why isn't there a Z move on line N124?

Because I have helix entry turned off

[Matthew Hajicek - Singularity]

 

This is for steel, so multiple passes and with a full profile tool.  Working backward, I do two passes at nominal, one 20% of the material away, and another an additional 30% of the material away.  The material is figured as the radial distance from the pilot hole to the major diameter of the thread.  Also, the larger the pilot hole is the better; I tend to use 50% thread in steels unless otherwise specified.

 

 

 

http://www.emastercam.com/board/topic/81688-thread-mill-38-npt-internal/#entry991921

THREADMILL TABLE 5-31-16.zip

[swanny]

Because I have helix entry turned off

Be careful defaulting to this type of toolpath. If you use a single point threadmill all will be good and you won't notice anything. But using a multi-flute threadmill, this will create a 1/4 turn of flat threads. I made this mistake already. That is how I know.

[Mick]

http://www.emastercam.com/board/topic/81688-thread-mill-38-npt-internal/#entry991921

 

Thanks for the information! I appreciate it.