Home Position

[Reddog34]

Hello,

I am running a Milltronics ML22 lathe with a Centurian 7 controll.

I am using Mastercam X3 with a MPFLAN post proccessor.

I need to use the tailstock most of the time.

The issue is that the code that I get from MPFLAN sends the tool post to the machine home I believe.

Which is beyond the tailstock.

 

The code I see is G28 U0. V0. W0. M05

What I think I need to see is G0 X15.0 Z0.0 M05

 

What do I need to edit and where is it located in MPFLAN?

Thanks!

Tim

[The Cathedral]

If you're using the default post, you don't need to change the post, just the control definition.

 

Open up your control definition, and go down to the "text" option. It will expand into suboptions. You need the first one, General Misc. Int/Reals.

 

You'll see that the first three have a definition in them:

 

Work Pos.

Abs/Inc

Ref. Return

 

Click into the box for the first one, and at the end of the text put in //1  

Do the same for the third one.

 

Save and exit.

 

This sets the default for every operation to 1. Post your program and it should be right.

[Reddog34]

Thank you!

I have a few more questions though.

1) Where do I set up the default home position for all tools?

2) This lathe is a flatbed, with a front mounted tool changer. If I define the home pos. in the Lathe tool setup box,  I have to put a minus sign in front of the X 7.5 value

     in order for the Toolpath Parameters page to show a positive number in the "Home Position" box. Do I need to change something in the machine axis page to correct this?

3) The post is outputting N110 G0 X15. Y 0. Z 0.  Why the Y 0.? This is only a two axis machine, and why does the post double the X value  from 7.5 to 15.0?

4)  When I run the program and an M01 prior to a toolchange is read, the machine  moves to a position about Z 2.9 and X at a diameter of about 3.00

     although my screen shows X7.5 Z 0.0?

5) At the machine I just gave it an MDI G0 Z15.0 and it moved to the correct location. The screen changed to X15.0 Z 2.8980

 

I know this is a lot. I really appreciate your help!

Tim

[The Cathedral]

Your default home position is set in the machine definition, in the machine axis combination tab. Keep in mind the numbers you'll see are Mastercam Top view numbers (like you're looking at the screen.) So Y is your lathe X, X, is your lathe Z, and Z is lathe Y.

 

I try not to define home positions with the tool. Leave it to the machine and you won't have that problem as long as it's set right; change the dropdown in the operation properties to Home Position > From Machine and it will stay the way you defined it in the step above. ^^

 

I believe you have a Y outputting because you must have an axis combination that includes a Y axis. Did you make this machine definition yourself? Is it just a generic machine definition? When I post using the MPLFAN post on a 2 axis, I get no Y; but if I use it on my Y-equipped Okuma's, I'll get a Y. This leads me to believe you need to check your axis combinations. As for the doubling, this is done in the post to convert numbers to diametrical. The home position isn't exempt, so the best thing to do is define your home position as half of what you want.

 

As for why your machine isn't moving to the numbers you type, that's beyond me. Make sure you're looking at the right offset; every machine has three "positions"- Machine position, Work Offset position, and Shift position. I can't really help you with this problem without actually seeing the machine work.

[Reddog34]

Hi,
So you know, I'm self taught on Mastercam X lathe, so when you say "Look at the right offset" I'm not really sure where to look! Given that, where do I find the three positions you refer to? Machine Position, Work Offset Position, and Shift Position.

This is the program I am getting when I post.
In this I have disabled all Lead in/Lead out moves, and I am using "Home Position from Machine".
In the Default Home Position Box I have
X 0.0
Y -7.50
Z 0.0

My Machine Axis Combination is set to Left/Lower.
In the Machine Configuration Box I have disabled the "Lathe Lower Turret Y axis button.
That is why I am no longer getting a "Y" dimension in the code I suspect.

%
O0000
(PROGRAM NAME - STUFFING BOX)
(DATE=DD-MM-YY - 21-07-14 TIME=HH:MM - 07:11)
(MCX FILE - M:\BLDG20\MASTERCAM\NC\ML22 FILES\T.MCX)
(NC FILE - M:\BLDG20\MASTERCAM\NC\ML22\STUFFING BOX.NC)
(MATERIAL - STEEL INCH - 1030 - 200 BHN)
N100 G20
(TOOL - 1 OFFSET - 1)
(STANDARD ROUGHER  INSERT - WNMG-432-MF2/EDP #27769)
( ROUGH FACE )
N110 G0 X15. Z0.
N120 G0 T0101 M06
N130 G97 S1200 M03
N140 G0 X2.2082 Z.01 M8
N150 G99 G1 X2. F.008
N160 X-.1425
N170 G0 X-.08 Z.0413
N180 X6.12
( ROUGH O.D. )
N190 Z.12
N200 X1.9319
N210 G1 Z-.24
N220 X2.
N230 G0 Z.12
N240 X1.8638
N250 G1 Z-.24
N260 X1.9519
N270 G0 Z.12
N280 X1.7957
N290 G1 Z-.0081
N300 G2 X1.82 Z-.0413 I-.0391 K-.0331
N310 G1 Z-.2213
N320 Z-.24
N330 X1.8838
N340 M9
N350 G0 X15. Z0. T0100
N360 M05
N370 M01
(TOOL - 2 OFFSET - 2)
(STANDARD O.D. FINISHING TOOL  INSERT - WNMG-331-MF2/EDP #27757)
( FINISH FACE )
N380 G0 X15. Z0.
N390 G0 T0202 M06
N400 G97 S1300 M03
N410 G0 X1.8113 Z.0156 M8
N420 G1 X1.78 Z0. F.005
N430 X-.08
( FINISH O.D. )
N440 G0 X1.7488
N450 G2 X1.8 Z-.0256 K-.0256
N460 G1 Z-.2056
N470 Z-.25
N480 M9
N490 G0 X15. Z0. T0200
N500 M05
N510 M01
(TOOL - 3 OFFSET - 3)
(5MM 0.016 RADIUS PROFILER  INSERT - LCMR 160504-0500-MC)
( ROUGH AND FINISH BACKSIDE O.D. )
N520 G0 X15. Z0.
N530 G0 T0303 M06
N540 G97 S1200 M03
N550 G0 X2.2 Z-.9372 M8
N560 G1 X1.41 F.005
N570 G0 X2.2
N580 Z-1.0788
N590 G1 X1.41
N600 X1.4666 Z-1.0505
N610 G0 X2.2
N620 Z-.7957
N630 G1 X1.41
N640 X1.4666 Z-.824
N650 G0 X2.2
N660 Z-1.2203
N670 G1 X1.39
N680 G0 X2.2
N690 Z-.6541
N700 G1 X1.41
N710 X1.4666 Z-.6824
N720 G0 X2.2
N730 Z-1.3619
N740 G1 X1.39
N750 X1.4466 Z-1.3336
N760 G0 X2.2
N770 Z-.5126
N780 G1 X1.41
N790 X1.4666 Z-.5409
N800 G0 X2.2
N810 Z-1.5034
N820 G1 X1.39
N830 X1.4466 Z-1.4751
N840 G0 X2.2
N850 Z-.402
N860 G1 X1.41
N870 X1.4666 Z-.4303
N880 G0 X2.2
N890 Z-1.645
N900 G1 X1.3793
N910 G0 X2.2
N920 Z-1.65
N930 X2.
N940 G1 X1.34
N950 Z-1.647
N960 X1.348
N970 G3 X1.38 Z-1.631 K.016
N980 G1 Z-1.466
N990 Z-1.1958
N1000 G3 X1.4 Z-1.181 I-.006 K.0149
N1010 G1 Z-1.016
N1020 Z-.401
N1030 G2 X1.408 Z-.397 I.004
N1040 G1 X1.748
N1050 G3 X1.8 Z-.371 K.026
N1060 G0 X1.83
N1070 M9
N1080 G0 X15. Z0. T0300
N1090 M05
N1100 M01
(TOOL - 7 OFFSET - 7)
(0.161 PARTOFF TOOL  INSERT - 150.10-4N-16,TGP45)
( PART OFF )
N1110 G0 X15. Z0.
N1120 G0 T0707 M06
N1130 G97 S1000 M03
N1140 G0 X1.864 Z-1.5203 M8
N1150 X1.5214
N1160 G1 X1.38 Z-1.591 F.003
N1170 G2 X1.34 Z-1.611 I-.02
N1180 G1 X-.02
N1190 G0 X1.58
N1200 M9
N1210 G0 X15. Z0. T0700
N1220 M05
N1230 M30
%

As you can see, the code sends the tool to X15.0 Z 0.0 just like I want, however in actuality at the end of every operation the tools back off to a position that varies from X 3.4941 to X 4.4752 and Z 2.4219 to Z 2.9020. It's as if there is an intermediate position the tools go to before they go to X 15.0 Z0.0.

Added to that, the actual "Tool Change Position" is X 17.1004 Z 2.9020.
This also sends the cross slide towards the tailstock.

 

Is it possible that when Mastercam cancels the tool offset with the line "T0100", that this is what the intermediate step is?

Thanks again! Your input thus far has been very helpful!
Tim

[The Cathedral]

Hi,

So you know, I'm self taught on Mastercam X lathe, so when you say "Look at the right offset" I'm not really sure where to look! Given that, where do I find the three positions you refer to? Machine Position, Work Offset Position, and Shift Position.

 

This is the program I am getting when I post.

In this I have disabled all Lead in/Lead out moves, and I am using "Home Position from Machine".

In the Default Home Position Box I have

X 0.0

Y -7.50

Z 0.0

 

My Machine Axis Combination is set to Left/Lower.

In the Machine Configuration Box I have disabled the "Lathe Lower Turret Y axis button.

That is why I am no longer getting a "Y" dimension in the code I suspect.

 

 

As you can see, the code sends the tool to X15.0 Z 0.0 just like I want, however in actuality at the end of every operation the tools back off to a position that varies from X 3.4941 to X 4.4752 and Z 2.4219 to Z 2.9020. It's as if there is an intermediate position the tools go to before they go to X 15.0 Z0.0.

 

Added to that, the actual "Tool Change Position" is X 17.1004 Z 2.9020.

This also sends the cross slide towards the tailstock.

 

Is it possible that when Mastercam cancels the tool offset with the line "T0100", that this is what the intermediate step is?

 

Thanks again! Your input thus far has been very helpful!

Tim

 

What I meant was, make sure you're looking at the right offset on your machine, not in Mastercam. The problems you're describing now all seem machine related. The tool change position is machine related and you should be able to change that in your work offset setup on the machine. I'm only familiar with Okuma lathes and we change our tool change position all the time. However I do notice that you have tool change codes on a stand-alone block; on the Okumas you have to have a Z position call on the same block as a tool call. So it looks like this:

 

G0 Z.1 T070707 M6

 

I also see you have no absolute or incremental commands.

 

It's possible that the tool offset cancel is causing the extra step. You're going to have to reference the programming manual for your machine to find the proper way it needs to be programmed. Since I have no experience with your machine I can't tell you what to change. If you can tell me exactly how it is supposed to be written, I can help you make the changes.

[Reddog34]

Thanks!

I contacted Milltronics about this. They suggested I manualy edit the program in the beginning with a line PB81=2

This turns off the trig help at the controller.

Then a line just before the M30 PB81=0

to turn it back on.

I,ll let you know how I make out!

Tim

[Reddog34]

Hello again,

Just a few other things.

This is a flatbed front turret lathe.

In the General Machine Parameters page,

for this machine which default cplane should I be using?

And in the window "Update wcs using"

None

Top

Lathe Z=World Z

 

As it stands now when I look at the Mastercam screen, in the lower left corner

is a set of coordinates with a x+ at the top of and a Z- on the right side.

Is this the way it should look?

Thanks!

Tim

[The Cathedral]

Hello again,

Just a few other things.

This is a flatbed front turret lathe.

In the General Machine Parameters page,

for this machine which default cplane should I be using?

And in the window "Update wcs using"

None

Top

Lathe Z=World Z

 

As it stands now when I look at the Mastercam screen, in the lower left corner

is a set of coordinates with a x+ at the top of and a Z- on the right side.

Is this the way it should look?

Thanks!

Tim

 

Your default WCS, T, C plane should all be Top. The reason you see the X+ and Z- is because you have your Cplane set to lathe radius.

 

This is fine, as long as the directions match the way you machine. I personally never use those planes, but it makes it easier for beginners to think about how their part is oriented.

[Satyajeet Sahoo]

Hello everyone, I have a little issue with my post processor. My machine is dmu 50 & the controller of heidenhan. While I am doing multi axis programming, it is not showing the same result in posting the programme what is showing in mastercam. Means if I am doing a single multi axis programme in mastercam with less retract,  it is showing N number of retract  to home position  & again taking the position. Please give me some solution as I am totally locked here how to solve the issue.

[#Rekd™]

You will need to attach a ziptogo file that includes the Mastercam file and the post processor. Once it is proven to be from a legitimate user not a pirate someone will help you.