MCX control setting or post issue...... G3 or G41 line

[honeybunches]

I posted yesterday and we are still trying to figure this out so we can move on. We have one post we worked on some time ago and works fine but does not support subs. We have two other posts that support subs and look wonderful but when posting out any type of Helical path, and probably others for that matter, we end up with a G3 on the G41 line and the machine will not use it. I have tried just deleting the G3 on that line and it will just move to the next and error out. I am trying to determine if this is an MCX settings issue or a post issue. One post was specifically designed for a Haas but was given to us so no support for it.

 

(this code does not work)

 

N150 T03 M6 ( )

N160

N170 G0 G90 G54 X2.339 Y-1.3 S7500 M3

N180 G43 H03 Z1.

N190 Z.6

N200 G17 G1 Z.5 F200.

N210 G3 G41 D03 Z.32 R-.57 F90.

N220 G3 Z.14 R-.57

N230 G3 X1.964 Y-1.8356 Z-.005 R-.57

N240 G3 X2.339 Y-1.3 R.57

N250 G3 X1.964 Y-1.8356 R-.57

N260 G3 X2.0363 Y-1.7494 R.1125

N270 G1 G40 X2.0364 Y-1.7485

N280 G0 Z1.

 

 

(this code works great)

 

N104 T3 M6

N106 G0 G90 G55 X2.339 Y-1.3 S7500 M3

N108 G43 H3 Z1.

N110 Z.6

N112 G1 Z.5 F200.

N114 G3 X1.199 Z.41 I-.57 J0. F50.

N116 G41 D3 X2.339 Z.32 I.57 J0.

N118 X1.199 Z.23 I-.57 J0.

N120 X2.339 Z.14 I.57 J0.

N122 X1.199 Z.05 I-.57 J0.

N124 X1.964 Y-1.8356 Z-.005 I.57 J0.

N126 X2.339 Y-1.3 R.57

N128 X1.199 R.57

N130 X1.964 Y-1.8356 R.57

N132 X2.0363 Y-1.7494 R.1125

N134 G1 G40 X2.0364 Y-1.7485

N136 G0 Z1.

 

 

Both paths are identical. I am pretty sure each post will call up it's own machine definitions so thinking we have have something setup wrong but not sure.

[Guest]

can you create a zip to go file with a part that outputs this way along with the post and defs?

 

Either put it on the FTP or email it and I'll have a look at your settings and post to determine what is happening.

[gcode]

Personally, I wouldn't run either of those toolpaths whether they worked or not..

Turning cutter comp on with G02 or G03 is asking for trouble.

You are lucky the machine is erroring out..

Many machines would just wreck your part with either toolpath..

If you are usingin Contour for your helicmill toolpaths use a small tangent leadin- followed

by an arc.. do the same with the lead out..

An easier solution is to use helix-mill in

the circle toolpaths.. and check the

Start at Center.. and use a 90° entery arc

your helixmill toolpaths should look like this

 

G1 Z15.01 F3.4

G41 D19 X-3.7131 Y.0275

G3 X-3.7406 Y0. J-.0275

Z14.97 I.055

Z14.93 I.055

Z14.89 I.055

Z14.85 I.055

Z14.81 I.055

Z14.77 I.055

Z14.73 I.055

X-3.6856 Y.055 Z14.7 I.055

J-.055 F1.7

X-3.7131 Y.0275 J-.0275

G1 G40 X-3.6856 Y0.

G0 Z15.5

 

note both G41 and G40 are on G1 lines..

G3G41 is asking for trouble

[honeybunches]

John, I emailed you. Let me know if you get it.

 

 

I am told that the older Haas we are running may be more forgiving than the newer controls so the code above that runs may still not work on a newer one because of the I J motion with the G41. Seems to come in fine for now but I also do not have any wear offset in my tables right now.

 

Makes me wonder if these are all post issues or if there is a setting issue in MC. I have tried helix and contour paths. I was trying to use helix because it allows finish feed rate control at the bottom of the pass which contour does not have. It would sure be nice to have more adjustability in feed rates... Would be nice to say "hey, slow down for that corner up there" but maybe that is what look ahead is for....

[Superman]

Modify your post to place errors on-screen that G3 G41 are being posted

Sorry I didn't explain

 

in the "error" section add

code:

---

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

---

and in the "Motion NC output" section,

modify the arc output to detect that G2/G3 has cutter comp (take-up or cancel) on the same line

code:

---

 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

---

This ensures that the NC-program has cut-comp on and off on lines only

[Guest]

First things being first, I would NOT be turning on cutter comp on an arc move, bad idea because it works OK in one condition does not mean machine/tool/cutter/geometry will like it in all. There is a reason why "most" machines will not allow cutter comp to be engaged/disengaged on arcs moves.

 

I created a helix bore with the post you provided and got this

code:

---

N1 G80 G40 G0 G20

T01 M6 ( 1/2 FLAT ENDMILL )

G0 G90 G54 X0. Y.404 S1069 M3

G43 H01 Z.25

Z.1

G17 G1 Z0. F15.

G41 D01 Y0. F25. <-------------

G3 Y.8079 I0. J.404

G3 Y-.8079 Z-.125 I0. J-.8079

G3 Y.8079 Z-.25 I0. J.8079

G3 Y-.8079 Z-.375 I0. J-.8079

G3 Y.8079 Z-.5 I0. J.8079

G3 Y-.8079 Z-.625 I0. J-.8079

G3 Y.8079 Z-.75 I0. J.8079

G3 Y-.8079 Z-.875 I0. J-.8079

G3 Y.8079 Z-1. I0. J.8079

G3 Y-.8079 I0. J-.8079 F7.5

G3 Y.8079 I0. J.8079

G3 G40 Y0. I0. J-.4039

G0 Z.25

M5

G0 G28 G91 Z0

G90 G129 X0. Y0.

G54

M30

---

A nice clean comp on move using perpendicular entry.

 

Then trying a Contour Ramp using a perpendicular entry, I got this

 

code:

---

N1 G80 G40 G0 G20

T01 M6 ( 1/2 FLAT ENDMILL )

G0 G90 G54 X-.5329 Y0. S1069 M3

G43 H01 Z.25

Z.1

G17 G1 Z0. F15.

G41 D01 X-.7274 Y.1945 F25. <------------

G3 X-.8079 Y0. I.1945 J-.1945

G3 X.8079 Z-.125 I.8079 J0.

G3 X-.8079 Z-.25 I-.8079 J0.

G3 X.8079 Z-.375 I.8079 J0.

G3 X-.8079 Z-.5 I-.8079 J0.

G3 X.8079 Z-.625 I.8079 J0.

G3 X-.8079 Z-.75 I-.8079 J0.

G3 X.8079 Z-.875 I.8079 J0.

G3 X-.8079 Z-1. I-.8079 J0.

G3 X.8079 I.8079 J0.

G3 X-.8079 I-.8079 J0.

G3 X-.7274 Y-.1945 I.275 J0.

G1 G40 X-.5329 Y0.

Z-.9

G0 Z.25

M5

G0 G28 G91 Z0

G90 G129 X0. Y0.

G54

M30

---

So, IMO anyway it is a user issue, not a post issue.

[honeybunches]

WOW John, I don't know what to say at this point. Is there any settings to check in MCX that would force code like I posted above? Now I am really scratching, wondering where I am going wrong here.

 

By the way John, did you get a chance to look at that Z+2.0" that is applied when using multi-offsets? I have been down and back in the post trying to to find that code.

[gcode]

quote:

---

Is there any settings to check in MCX

---

Circlemill/helixbore.. check "start at center"

set entry arc to 90°

 

if you are using contour/ramp for helix bore

set you lead-in/lead out

tangent ... and a small value + a small arc

[Justin Beebe at Folsom Tool]

Viper,

 

It's controlled in your lead in/out settings. Do you have Lead in/out turned on?

[Midwest]

This is what I get using Wear and a Perp leadin/leadout.

 

mpMaster post.........for our Haas

 

 

%

O0200 (T)

(MASTERCAM - X)

(MCX FILE - T)

(POST - MPMASTER)

(MATERIAL - STEEL INCH - P20 - 175 BHN)

(PROGRAM - T.NC)

(DATE - APR-25-2009)

(TIME - 11:10 AM)

(POST DEV - IN-HOUSE SOLUTIONS)

(T1 - 1.0 DIA 3 FLUTE BULLNOSE - H1 - D1 - D0.9960" - R0.0310")

G00 G17 G20 G40 G80 G90

(1.0 DIA BULLNOSE 3 FLUTE G41 USING WEAR)

T1 M06 (1.0 DIA 3 FLUTE BULLNOSE)

(MAX - Z1.)

(MIN - Z-.4)

G17

G00 G90 G54 S2387 M03

X-.402 Y0.

G43 H1 Z1.

Z.05

G94 G01 Z0. F18.

G41 D1 Y.1 F36.

G03 X-.502 Y0. I0. J-.1

X0. Y-.502 Z-.025 I.502 J0.

X.502 Y0. Z-.05 I0. J.502

X0. Y.502 Z-.075 I-.502 J0.

X-.502 Y0. Z-.1 I0. J-.502

X0. Y-.502 Z-.125 I.502 J0.

X.502 Y0. Z-.15 I0. J.502

X0. Y.502 Z-.175 I-.502 J0.

X-.502 Y0. Z-.2 I0. J-.502

X0. Y-.502 Z-.225 I.502 J0.

X.502 Y0. Z-.25 I0. J.502

X0. Y.502 Z-.275 I-.502 J0.

X-.502 Y0. Z-.3 I0. J-.502

X0. Y-.502 Z-.325 I.502 J0.

X.502 Y0. Z-.35 I0. J.502

X0. Y.502 Z-.375 I-.502 J0.

X-.502 Y0. Z-.4 I0. J-.502

X0. Y-.502 I.502 J0.

X.502 Y0. I0. J.502

X0. Y.502 I-.502 J0.

X-.502 Y0. I0. J-.502

X-.402 Y-.1 I.1 J0.

G01 G40 Y0.

G00 Z1.

M05

G91 G28 Z0.

G28 X0. Y0.

G90

M30

%

 

 

Have you tried using Wear?????

 

 

 

 

 

 

quote:

---

One post was specifically designed for a Haas but was given to us so no support for it.

---

Try the mpmaster post.....

 

 

HTH

 

 

[honeybunches]

I am an idiot and sorry to waste anyone's time. After doing some testing, I have determined that I must create lead in/out paths to have one straight line in them. This gives the G41 a line move to start with. What I had before was a continuous arc from center of circle, to the outside cutpath. By just adjusting to 90*, it created a line move out, then into a nice lead in arc with G3. I am guessing this code will work much better. You guys have made my day!

[Guest]

quote:

---

I have determined that I must create lead in/out paths to have one straight line in them.

---

You're using control comp, aren't you?

 

You're ultimately, I'm gonna got killed for this I know, you're ultimately better off using computer and wear for those times when you need adjustment in your tool.

[Justin Beebe at Folsom Tool]

John,

 

You will hear no complaints from me for your advice about the computer and wear comp.

[honeybunches]

I am using wear comp. I was using computer because we had not had any need to adjust paths. Now we do and this is what started the snow ball. Just needed to adjust a cutter path by a few thou. I will hopefully get this code on a machine later today or tomorrow to see if we can adjust the path. We had problems before where the machine would run until I put any non-zero number in the comp tables, then it would alarm out.

 

John, I was going to ask about that Z move (+2.0") when you use multi-offsets with that post I sent. The post commands extra Z clearance when moving to the next offset. Did you see a place to adjust that? I could not find it at ALL but probably looking in the wrong spot.

[honeybunches]

Well, it looks like I am still outputting R code for these helix paths and I think it is causing my latest errors. I would like to get back to I J paths. How would I accomplish this? I tried going into the control def and changing things there but it said it could not apply it. I just tried changed "do not break arcs" to "180*".

[Justin Beebe at Folsom Tool]

Viper

 

You change R to IJK in your control definition.

There are two ways to change your control definitions. One way changes them just for the local mastercam file you are working on and one way changes them permanately for all future mastercam files.

 

To make the change for a single mastercam file do the following:

 

1. Open your operation manager

2. Click on "Files"

3. Under machine-toolpath copy click "Edit"

4. Click the "edit the control definition icon"

5. Click "Arc"

6. Under Arc center type use the drop down arrow and change "Radius" to "Delta Start to Center"

For XY Plane, XZ Plane, And YZ Plane.

7. Select the green check marks to exit

 

To make the change stick for all future sessions of mastercam use the

 

1. Settings

2. Machine definition manager

3. Click the green check mark

4. Click the "edit the control definition icon"

5. Follow the same steps I listed above

[Guest]

First off, I am going to say I WOULD NOT change this. IMO there is too much happening with subs and all to be overly concerned about an "extra" Z call.

 

If you want to know where this come from

 

code:

---

N1 G80 G40 G0 G20

T01 M6 ( 1/2 FLAT ENDMILL )

G0 G90 G54 X-.475 Y.3889 S1069 M3

G43 H01 Z2.

M97 P100

G0 Z4.

G55 X-.475 Y.3889

Z2.<---------

M97 P100

G0 Z4.

G56 X-.475 Y.3889

Z2.<---------

M97 P100

G0 Z4.

G57 X-.475 Y.3889

Z2.<---------

M97 P100

G0 Z4.

G58 X-.475 Y.3889

Z2.<---------

M97 P100

M5

G0 G28 G91 Z0

G90 G129 X0. Y0.

G59

M30

---

it is from this postblock, the noted line

 

code:

---

pwcs_call  # WCS Call

if sub_flag1 = 1, n$, psg00, *z_sub_clr, e$

if sub_flag1 = 1, n$, sgwcs, *xr$, *yr$, e$

if sub_flag1 = 1, n$, *zr$, e$ <--------------

if fan_haas = 1, n$, "M97", subno, e$

else, n$, "M98", subno, e$

sub_flag1 = 1

---

Again, this isn't anything I'd change.

[honeybunches]

You guys have been a tremendous amount of help. I think I have everything tuned about right "except" (and only a convenience thing) it would be nice to call the specific offsets I want to use instead of the post automatically starting at G54 and counting up from there.

 

John, I guess I would ask you this question more or less because you have the post. Is there an easy way to tweak it to allow me to assign specific offsets? ie, G54, G56, G58, G110 ? Seems I will still have to adjust things in the program unless I can tell it which to use. This might take a bunch of tweaking though. I am not sure.

 

I did edit out that Z+ move but highlighted it and may add a second post with that move since I do understand what you are saying and it could save a crash some day or at least save some hand edits.

[Philcott]

Viper1,

 

You can set your work offset by going to the toolpath parameter page, click Planes, check the box beside work offset and by putting a 1,2,3,4 etc. you can set the offset to use.

 

0 is G54, 1 is G55 and so on.

[honeybunches]

Thanks but our post creates the multi-offsets and I tried inputting in planes but did not affect my posted code. I will study the post a bit today and see if I can understand how to do this. Our offsets are a function of the misc values and there is only an input now for how "many" offsets and not "which" offsets I want to use. Obviously I can just change these in the posted file but if I am running 4 offsets and 20 tools, that can take a while to change.

[NickUsaMi]

Lead in/out (in the toolpath Parameter) must have minimal value in "Line in" and "Line out"