No tool comp Okuma OSP200 X3

[Brian L.]

Ok, so I'm finally getting the hang of mastercam and the mpokuma post. Ive gotten everything i need to work except for in-machine tool comp.

 

I have changed the tool comp options in mastercam from "computer" to "wear" with no change in the posted code. Changing the D offset on the machine has no effect on the part dimensions. The code and below is a snippet of what is produced when posting. (no tool comp, block delete on)

 

Your insight is very much appreciated.

 

 

code:

---

 $CUBE.MIN%

(MASTERCAM - X)

(MCX FILE - G:MY DOCUMENTSCUBE.MCX)

(POST - MPMASTER_OKUMA)

(MATERIAL - ALUMINUM INCH - 2024)

(PROGRAM - CUBE.MIN)

(DATE - JUN-18-2009)

(TIME - 9:31 PM)

(POST DEV - IN-HOUSE SOLUTIONS)

(T4 - 1/2 FLAT ENDMILL - H4 - D4 - D0.5000")

(T1 - 1/4 FLAT ENDMILL - H1 - D1 - D0.2500")

(T3 - 1/4 BALL ENDMILL - H3 - D3 - D0.2500" - R0.1250")

(T2 - 1/8 BALL ENDMILL - H2 - D2 - D0.1250" - R0.0625")

(OVERALL MAX - Z1.)

(OVERALL MIN - Z-1.51)

N10 G00 G17 G20 G40 G80 G90

N12 G30 P1

/ N14 M01

/ N16 S7334 M03

/ N18 G116 T4 ( 1/2 FLAT ENDMILL)

N20 (MAX - Z.25)

N22 (MIN - Z-1.51)

/ N24 G15 H1

/ N26 G00 G17 G90 X-.3912 Y-1.3417 S7334 M03

/ N28 G56 H4 Z.25 T1

/ N30 Z.1

/ N32 G94 G01 Z0. F6.42

/ N34 G03 X-.26 Y-.75 I-1.2688 J.5917 F58.67

/ N36 G01 Y0. Z-.0098

/ N38 X-.2592 Y.0199 Z-.0101

/ N40 X-.257 Y.0397 Z-.0103

/ N42 X-.2532 Y.0592 Z-.0106

/ N44 X-.2479 Y.0784 Z-.0109

/ N46 X-.2412 Y.0972 Z-.0111

/ N48 X-.233 Y.1154 Z-.0114

/ N50 X-.2235 Y.1329 Z-.0117

---

[35K chipper]

no G41 or G42. got to have for wear comp!

 

35k

[Brian L.]

Well i understand that... but now I'm trying to figure out why its not there

 

I think I may be onto something here... Browsing through the mpmaster post I found this in the user-defined variables :

 

code:

---

  comp_type    : 0     #Cutter compensation type - 0=computer, 1=control, 2=wear, 3=reverse wear, 4=off

---

Now my question is.. do i have to set this manually the toolpath parameters do this automatically?

[Slepydremr]

Out of curiosity..What type of operation are you starting that first tool with? I'm just wonder cause it is feeding in all 3 axis like the beginning of a pocket or something and if it is a pocket the G comp will not get turned on till the last pass.

 

also did you do a search of all G-code to see if a G41 is turning on later?

 

The toolpath parameters should be what always controls the Comp

[Brian L.]

The first operation is a Ramp Contour. It will run around a 1.5" square part at .05 depth until 1.51" with a .01" finish cut. G41 is not turned on anywhere else in the program. I managed to get comp to post on the first move and it gives me the "cutter comp applied on arc move" error message. I had it set to us entry/exit but it was not necessary. After turning it off it posted without error and i got the following.

 

It seems that ive answered my own question here???

 

code:

---

  (OVERALL MAX - Z1.)

(OVERALL MIN - Z-1.51)

N10 G00 G17 G20 G40 G80 G90

N12 G30 P1

/ N14 M01

/ N16 S7334 M03

/ N18 G116 T4 ( 1/2 FLAT ENDMILL)

N20 (MAX - Z.25)

N22 (MIN - Z-1.51)

/ N24 G15 H1

/ N26 G00 G17 G90 X-.26 Y-1.5 S7334 M03

/ N28 G56 H4 Z.25 T1

/ N30 Z.1

/ N32 G94 G01 Z0. F6.42

/ N34 G41 D4 Y0. Z-.0196 F58.67

/ N36 X-.2592 Y.0199 Z-.0199

/ N38 X-.257 Y.0397 Z-.0202

/ N40 X-.2532 Y.0592 Z-.0204

---

[Slepydremr]

It looks as though you have.

 

Try doing a simple 2d contour with no ramp.

 

Also when using leadin-lead out and wear cutter comp. you must have a lead in line with any arc you're using. It can be a pretty short line but you're first move must always be linear.

[Brian L.]

I got it now I think. I did a few searches after pinpointing the error and realized that a linear move is all I need. Lead in/out is not necessary for this path but this is good to know for future reference.

 

I prefer to use Ramp instead of depth cuts.... I guess it makes me feel better about choosing to do something CNC instead of manually.

 

Off topc but deffinately due to being new to mastercam x....

 

I use canned text to put an M01 before each operation.... it puts it before EVERY pass on depth cuts. While this is good for proving out a program, it sucks if i just wnat to use an M01 to stop for clamp swaps and such. Any ideas?

[Greg Williams]

I see you use G116 for the tool change, Good choice

 

Just out of interest, Why is there a backslash on every line / ?

[Superman]

Don't forget that Okuma's require a line to take cutter comp on, and also to cancel.

 

Lead ins / outs must have a line ( perpendiculr or tangent ), the arc is optional, but is a good idea to use in many situations as is allows an angled and smoother approach to the contour.

 

No lead in/out means the tool plunges adjacent to the start point of your contour.

 

Now over-riding all this is the lead in / out must not cross the actual toolpath or it will be skipped

 

eg a 1" bore done with a 1/2" cutter, and wear comp

-using a 1/4" arc,90° sweep, tangent line 1/4" long-------will not allow the lead in/out

-using a 0.20" arc, 90° swwep, perpendicular line 0.20"" long-------will allow the lead in/out

 

If using cut-comp in the "Control", the lead in/out lines must be bigger than the tool radius, arcs also.

[Colin Gilchrist]

What are your settings for the Opstop?

 

All canned text outputs have three options:

 

1. Before

2. With

3. After

 

Depending on how your post is setup you would normally just use "before" with your Opstop canned text and this would give you an M01 before the toolchange.

 

You need to take a look at how your post is configured though.

 

Some posts have a switch in the post to toggle the M00/M01 options before a toolchange. This is independent of canned text.

 

Some posts use a Misc. Integer to control M00/M01 output before the toolchange.

 

Try reading the header of your post. Most post processors have notes at the top about how the post is setup and how to control it using the Misc Integers...

 

HTH,

[Brian L.]

Greg: The post was set up to use G116 by default but I definitely find it more convenient. Also, the is optional block delete. I am using this to toggle on off the first two operations. It is an outer contour and a facing operation that only needs to be done once. I am running the same program for a 6 sided part so all i have to do is run the program once, then flip the part and turn on block delete.

 

Superman: The G41 is called, D(X) and then at the bottom of the program it cancels with G40(not shown). Looks good to me....

 

quote:

---

If using cut-comp in the "Control", the lead in/out lines must be bigger than the tool radius, arcs also.

---

Will mastercam warn you if you dont have large enough arcs/lines?

 

Colin: I Have Ostop set for on before. I need to look at the post and play around with mastercam a bit more posting simple operations to see what each setting does.

[Brian L.]

RE: Ostop It seems to work fine but when i turn on the Ostop on the control the coolant does not come back on. Also, is there a way in mastercam to tell the machine to go home on an M01 instead of just sitting over the part?

[Superman]

A couple of mods to the post for comp on arcs

 

add in the "Error Messages" section

sworkoffseterror "ERROR - NO WORK CO-ORD SYSTEM APPLIED"

sspeederror "ERROR - RPM NOT SET CORRECTLY ?"

speck1error "ERROR - NO PECKS SET FOR DRILLING"

scutcomperror "ERROR - CUTTER COMP STARTS / FINISHES ON AN ARC"

 

If the other error detects appeal to you, give us a hoy

 

 

Modify "NC Motion" to detect that comp is started before doing arcs

pcirout #Output to NC of circular interpolation

if prv_cc_pos$ <> cc_pos$, result = mprint (scutcomperror), "ERROR-CUTTER COMP"

pcan1, pbld, n$, `sgfeed, sgplane, sgcode, sgabsinc,

pxout, pyout, pzout, pcout, parc, feed, strcantext, scoolant, e$ #pccdia removed