More Threadmill help

[Kyle M]

HI all, I posted my program on the ftp

MCX_MR2_or Earlier_Files/THREAD MILL HOUSING MANIFOLD.MCX I am pretty new at this so any help would be appreciated. My new problem is. When I run the program on my test part the thread mill isn't cutting or just touches the boss.

I am thread milling a 1"-14 25.3492mm(.998in) boss. I picked the circle chain on the boss. I picked a dove tail tool and set it to 20.066(.79in) diameter. I got that by measuring the tool then confirming it on the Vardex web sight. I set the active teeth to 8. Thread depth to -18. Thread pitch to 1.81428 (thanks iowajim62 for the refresher) Selected helical entry/exit for top and bottom. Selected OD thread set minor thread diameter to 1.81428(.930in) from my Machinery's Handbook. Selected right hand thread and machine top to bottom.

 

I am using the first release of MCX. Material is AL and I am using a Vardex 3/8 thread mill TMC0753

 

Thanks for any Help,

Kyle

[#Rekd™]

Hi Kyle,

 

The active teeth should match the cutter? (I am at home and can not check your file) Go into edit tool and check the angle, should be 180 deg. Instead of picking the circle create a point and pick the point, this gives you options. Then choose starting from the bottom or top.

 

Good luck.

 

John

[Kyle M]

Maybe my file isn't on there anymore I uploaded it ,but it isn't showing through the link on the top browsing bar. When I can log back onto the server I will try to re upload it

[#Rekd™]

Hi Kyle,

 

I looked at your file and it appears that you are using a dovetail cutter? I don't think this will work but you can use a single point tool but set your active teeth to 1 instead of 8.

 

John

[Kyle M]

Thanks for the replys. I used that link to set it up initially. I get the same results of the tool not cutting, just skimming the part, no matter what tool I use. I first started out with a flat endmill. It was my understanding that the tool that you picked only effected the verify, and not the code that went to the machine.

[Guest]

Kyle,

 

Your problem of skimming is this.

 

You chose the "circle" as your geometry, when you pick a circle, the cycle automagically inherits the diameter to cut, your is the major diameter, notice your dialog box is greyed out.

 

 

I edited your path, reselected geometry and used the window point method, I windowed the point you have at the center, notice now I can type in the minor diameter and no longer just "skim" the OD.

 

[Kyle M]

John and John, Thanks for taking the time to look at my program, I did what you suggested, but I am still getting the same thing.

 

I set minor thread diameter to 23.622(.930in)

[iowajim62]

Kyle,

you repicked a point for geo?

you reset your minor thread dia to 23.622?

 

try changing to wear comp instead of computer

 

also try absolute instead of incremental

[Kyle M]

Jim,

I just double checked every thing, changed the wear comp, and changed to absolute. There is no change. I tried changing the variables by large amounts like tool dia and minor diameter. I can see no changes with backplot. The tool still follows the outside of the boss. I don't understand what controls the tool depth. It seems like minor diameter would control how deep the tool cuts the threads.

 

Thanks,

Kyle

[crazy^millman]

quote:

---

I don't understand what controls the tool depth. It seems like minor diameter would control how deep the tool cuts the threads.

---

No the thread depth on the options controls this.

 

HTH

[Kyle M]

Thread depth seems to be controlling how deep in Z the tool cuts, or how far down the boss it cuts. I'm Trying to figure out how to control the depth in x/y the thread mill cuts into the boss. It seems what ever i change the tool just skims the outside diameter of the boss.

 

Thanks for the help

Kyle

[crazy^millman]

Let me get this straight you change the geometry to point and now have a number? In changing this number it does not cut more if you make it smaller and it does not cut less if you make it bigger???

 

Here is one with a 1.81 dia using OD thread. I took out entry/exit arc and Helical entry/exit at top and bottom of thread so we can just see the code for the threadmill toolpath itself.

 

code:

---

N100 G0 G17 G20 G40 G80 G90

N110 T239 M06 ( 1/2 FLAT ENDMILL)

N120 (MAX - Z.25)

N130 (MIN - Z-.6)

N140 G0 G54 X0. Y1.155 S1069 M3

N150 G43 H0 Z.25

N160 G94 G1 Z.1 F6.42

N170 G2 X1.155 Y0. I0. J-1.155

N180 X-1.155 Z.0375 I-1.155 J0.

N190 X1.155 Z-.025 I1.155 J0.

N200 X-1.155 Z-.0875 I-1.155 J0.

N210 X1.155 Z-.15 I1.155 J0.

N220 X-1.155 Z-.2125 I-1.155 J0.

N230 X1.155 Z-.275 I1.155 J0.

N240 X-1.155 Z-.3375 I-1.155 J0.

N250 X1.155 Z-.4 I1.155 J0.

N260 X-1.155 Z-.4625 I-1.155 J0.

N270 X1.155 Z-.525 I1.155 J0.

N280 X-1.155 Z-.5875 I-1.155 J0.

N290 X-.9344 Y.6789 Z-.6 I1.155 J0.

N300 X.6789 Y.9344 I.9344 J-.6789

N310 G0 Z.1

N320 Z.25

---

Here is the same thing expect 1.71 dia OD thread.

 

code:

---

N110 T239 M06 ( 1/2 FLAT ENDMILL)

N120 (MAX - Z.25)

N130 (MIN - Z-.6)

N140 G0 G54 X0. Y1.105 S1069 M3

N150 G43 H0 Z.25

N160 G94 G1 Z.1 F6.42

N170 G2 X1.105 Y0. I0. J-1.105

N180 X-1.105 Z.0375 I-1.105 J0.

N190 X1.105 Z-.025 I1.105 J0.

N200 X-1.105 Z-.0875 I-1.105 J0.

N210 X1.105 Z-.15 I1.105 J0.

N220 X-1.105 Z-.2125 I-1.105 J0.

N230 X1.105 Z-.275 I1.105 J0.

N240 X-1.105 Z-.3375 I-1.105 J0.

N250 X1.105 Z-.4 I1.105 J0.

N260 X-1.105 Z-.4625 I-1.105 J0.

N270 X1.105 Z-.525 I1.105 J0.

N280 X-1.105 Z-.5875 I-1.105 J0.

N290 X-.894 Y.6495 Z-.6 I1.105 J0.

N300 X.6495 Y.894 I.894 J-.6495

N310 G0 Z.1

N320 Z.25

---

You will notice the X changed from X1.155 to X1.105. NOw if you want to take passes you use the mulitpass and decide on the amount.

 

Here is posted code for 4 cuts again just code no entry/exit or helical entry/exit at top and bottom of thread using 1.81 diameter and .01 pass.

 

code:

---

N110 T239 M06 ( 1/2 FLAT ENDMILL)

N120 (MAX - Z2.)

N130 (MIN - Z-.6)

N140 G0 G54 X.1875 Y0. S1069 M3

N150 G43 H0 Z2.

N160 Z.1

N170 G94 G1 Z-.5 F6.42

N180 G3 X-.1875 I-.1875 J0.

N190 X.1875 I.1875 J0.

N200 G1 Z-.4

N210 G0 Z2.

N220 X0. Y1.17 Z.25

N230 G1 Z.1

N240 G2 X1.17 Y0. I0. J-1.17

N250 X-1.17 Z.0375 I-1.17 J0.

N260 X1.17 Z-.025 I1.17 J0.

N270 X-1.17 Z-.0875 I-1.17 J0.

N280 X1.17 Z-.15 I1.17 J0.

N290 X-1.17 Z-.2125 I-1.17 J0.

N300 X1.17 Z-.275 I1.17 J0.

N310 X-1.17 Z-.3375 I-1.17 J0.

N320 X1.17 Z-.4 I1.17 J0.

N330 X-1.17 Z-.4625 I-1.17 J0.

N340 X1.17 Z-.525 I1.17 J0.

N350 X-1.17 Z-.5875 I-1.17 J0.

N360 X-.9465 Y.6877 Z-.6 I1.17 J0.

N370 X.6877 Y.9465 I.9465 J-.6877

N380 G0 Z.1

N390 Z.25

N400 X0. Y1.165

N410 G1 Z.1

N420 G2 X1.165 Y0. I0. J-1.165

N430 X-1.165 Z.0375 I-1.165 J0.

N440 X1.165 Z-.025 I1.165 J0.

N450 X-1.165 Z-.0875 I-1.165 J0.

N460 X1.165 Z-.15 I1.165 J0.

N470 X-1.165 Z-.2125 I-1.165 J0.

N480 X1.165 Z-.275 I1.165 J0.

N490 X-1.165 Z-.3375 I-1.165 J0.

N500 X1.165 Z-.4 I1.165 J0.

N510 X-1.165 Z-.4625 I-1.165 J0.

N520 X1.165 Z-.525 I1.165 J0.

N530 X-1.165 Z-.5875 I-1.165 J0.

N540 X-.9425 Y.6848 Z-.6 I1.165 J0.

N550 X.6848 Y.9425 I.9425 J-.6848

N560 G0 Z.1

N570 Z.25

N580 X0. Y1.16

N590 G1 Z.1

N600 G2 X1.16 Y0. I0. J-1.16

N610 X-1.16 Z.0375 I-1.16 J0.

N620 X1.16 Z-.025 I1.16 J0.

N630 X-1.16 Z-.0875 I-1.16 J0.

N640 X1.16 Z-.15 I1.16 J0.

N650 X-1.16 Z-.2125 I-1.16 J0.

N660 X1.16 Z-.275 I1.16 J0.

N670 X-1.16 Z-.3375 I-1.16 J0.

N680 X1.16 Z-.4 I1.16 J0.

N690 X-1.16 Z-.4625 I-1.16 J0.

N700 X1.16 Z-.525 I1.16 J0.

N710 X-1.16 Z-.5875 I-1.16 J0.

N720 X-.9385 Y.6818 Z-.6 I1.16 J0.

N730 X.6818 Y.9385 I.9385 J-.6818

N740 G0 Z.1

N750 Z.25

N760 X0. Y1.155

N770 G1 Z.1

N780 G2 X1.155 Y0. I0. J-1.155

N790 X-1.155 Z.0375 I-1.155 J0.

N800 X1.155 Z-.025 I1.155 J0.

N810 X-1.155 Z-.0875 I-1.155 J0.

N820 X1.155 Z-.15 I1.155 J0.

N830 X-1.155 Z-.2125 I-1.155 J0.

N840 X1.155 Z-.275 I1.155 J0.

N850 X-1.155 Z-.3375 I-1.155 J0.

N860 X1.155 Z-.4 I1.155 J0.

N870 X-1.155 Z-.4625 I-1.155 J0.

N880 X1.155 Z-.525 I1.155 J0.

N890 X-1.155 Z-.5875 I-1.155 J0.

N900 X-.9344 Y.6789 Z-.6 I1.155 J0.

N910 X.6789 Y.9344 I.9344 J-.6789

N920 G0 Z.1

N930 Z.25

---

If you will notice the X changes in increments of .005 like we want starting at X 1.17 then going down in .005 since we only see half of the helix you get have the value for the total .01 per pass to the root size you are looking for.

 

HTH

[c-hook]

I've always preferred thread milling using sub programs over mastercam. Not to say that mastercam doesn't do a good job. It it's just my preference, and works better for me in my situation. Using a sub makes it easy to modify at the control without having to repost anything and significantly shortens the whole thing as well.

 

Here is an example of how I usually thread mill.

 

G0 G90 G54 X1.5 Y0.

S1069 M3

/M8

G43 H1 Z1.

Z.1

G1 X1.17 F6.

M98P1L10

G90

G1X1.5M9

G0G91G28Z0

M30

 

O0001

G91

G2I-1.17Z-.0174

M99

 

 

I know there are several ways to create a thread milling program . For me this works nicely.If you need to change the diameter just change two X values, if you need more thread in the Z travel, just change the L value. Need to thread mill more than one location, add another XY.

 

Also works great for plung milling or any application where a helical entry is needed.

[Kyle M]

Thanks for the replys, but I still haven't found a solution. I still cant get the thread mill to cut it just skims around the boss.

 

I've updated the program on the FTP /MCX_MR2_or Earler_Files/THREAD MILL HOUSING MANIFOLD.MCX

 

These are my settings for 1"-14

 

Boss 25.3492(.998in)

Tool 20.066 (.79) Vardex 3/8 thread mill TMC0753

Active teeth 8

Thread pitch 1.81428

Comp type computer

OD thread selected

Minor thread DIA set to 23.4442(.923)

Right hand thread selected

Top to bottom machining direction.

 

What the heck am I missing?

Thanks for any help,

Kyle

[Chris Rizzo]

Hey Kyle!

 

Ok I figured it out. There is definitely a bug happening here.

 

- No matter what value you key in for the minor dia. the code output is identical. In other words that field is not working. The value it is "locking onto" and using is the diameter of your boss, which is 25.3492, and also what you selected (as solid). i think it is something to do with the solid point selection.

 

- The Fix. Draw an arc your minor dia 23.4442 and select THAT as your driving geo.

 

HTH

 

I'll submit the bug. My file is on ftp renamed:

THREAD MILL HOUSING MANIFOLDRIZZO.MCX however you can probably do it faster yourself than downloading

[Dave Ball]

Sometimes MC won't let go of the solid geometry, if you later decide it is the wrong size and pick a point, then try to use the Diameter field to input a value. Your able to enter a value but it is ignored and the original solid geometry size is used. I don't know why but it does. The only fix I have found is to select just the point not the arc center point and even then sometimes this doesn't work. Otherwise, delete the operation and start over ensuring that you select a point and not the solid geometry. I did however get your file to work correctly.

 

 

 

[ 08-06-2008, 10:10 PM: Message edited by: ShefferCNC ]

[Kyle M]

Great thanks alot Chris and ShefferCNC.

 

Chris, I'll be retaking your mastercam class this winter term if your still teaching it. See you then.

[Chris Rizzo]

Oh great Kyle, now I'll have to come up with all new parts to work on 'cause you know the old ones!

 

Really, it would be great to have you back. I hear a lot of other good people are interested in it already too.

[DaveR]

It appears to still be an issue in X3.

 

Had the same problem yesterday, was scratching my head all eve (boy do I have a sore head) over this.

 

 

Dave