Correcting the Mazak high speed implementation in MPMaster

[Joe788]

Oh post gurus, I bow before you for help fixing the Mazak G61.1 and G05P2 implementation in the new MPMaster post. (<--Just needed an excuse to use that new emoticon!)

 

Here's the problem.

 

MAZACC3D is turned on with G05P2, and off with G05P0. This is for 3D work. I just need it to turn ON, on it's own line, immediately before the first feed moves, and it needs to turn OFF (G05P0) before any comments.

 

So it needs to turn off and on with EVERY toolpath, not just once for each tool.

 

There are no special conditions for calling or cancelling. It just needs to turn on after the G43, and off immediately after the last feed move, before any comment, M05, M09, G91G28Z0, etc.

 

Any comment, M code, or G28 will cause an alarm.

 

Also, the current MPMaster defaults to 500ipm feed moves when the Mazak high speed code is applied. This is not necessary. G61.1 and G05 both allow rapids. Because of this high feed, I don't even use the Mazak high speed miscellaneous integer. I just have to hand add it. Well, this morning I'm working on a job that has dozen of 3D paths, so you can see why I need to get this working propertly.

 

I'm using a fresh download of MPMaster, with some very minor changes (Changing the VMC post to work on a Horizontal).

 

Code would look like this:

 

(COMPENSATION TYPE - COMPUTER)
T113M06(1.0 BALL MILL)
T17
(MAX - Z.5)
(MIN - Z-.8549)
(TOOLPATH - FINISHPARL)
(STOCK LEFT ON DRIVE SURFS = .001)
M08
G0G17G90G54B0X-1.7305Y-.7221S15000M03
G43H113Z1.25
Z-.1945
G05P2<------------------CALL HERE
G94G01Z-.2945F150.
X-1.7
X-1.6287Z-.2935
X-1.5715Z-.2897
.
.
.
.
.

Z.16
G01Z-.8549
X-.19Z-.374
G0Z1.25
G05P0  <--------CANCEL HERE
Z1.25
(RIGHT SIDE STRAGGLER)
(TOOLPATH - FINISHPARL)
(STOCK LEFT ON DRIVE SURFS = .0001)
X1.9087Y-.045
Z.6001
G05P2 <---------CALL AGAIN HERE
G01Z.4001
Y.005
Y.2575
Y.3075
.
.
.
.
.

[mayday]

+1

 

also need the smoothing option M820 through M830

I hand edit right after the G43 line. As of yet I dont think it needs turning off

[Joe788]

I've never sprung for the smoothing option. Have you ever noticed a difference between using just G61.1 with G05, vs using them with the smoothing as well? I've got a job here right now that could probably really benefit from it.

[mayday]

Big improvements in our 5 axis toolpaths with smoothing. Thats about the only time I use it. I have run it along with dynamic milling and it has helped maintain surface accuracy

[Joe788]

I might have to check that out. 3 axis paths are very fast and smooth with just G61.1 and G05 right now, but I'm always interested in going faster.

 

As for the post mod, I figure it's gotta be about a 5 minute job for somebody who understands the post language. Unfortunately, that somebody isn't ME. I put this into my old school MPMaster post before the days of machine and control defs, but even then it wasn't in the right spot. I put it in the retract block, so it canceled G05 before the retract, but that didn't do me any good when a tool was doing more than one 3D path.

 

In the old days, I just put this in the ptlchng block immediately after the G43:

 

if mi1$ = 1

pbld, n$ "G61.1,K70", e$

 

if mi3$ = 1

pbld, n$ "G05P2", e$

 

G61.1 worked fine, because I never cancel that anyways.

 

 

 

Misc Integer 7 seems unused, so I guess what I'd like to do now, is put:

 

if mi7$ = 1

pbld, n$ "G05P2", e$

 

...before the first feed line for each operation. And:

 

if mi7$ = 1

pbld, n$ "G05P0", e$

 

 

...after the last feed line for each operation. I don't know WHERE that is though.

[Joe788]

I think I've hand added about 150 G05P2 and G05P0s since starting this topic this morning.

[K2csq7]

Joe, first, I see your missing commas after your n$

pbld, n$, "G05P0", e$

 

And for your "after the last feed line for each operation. I don't know where that is though"

Do you know how to use the post debugger? You NEED to be able to use this for simple post mods... Its like trying to bang in a nail without a hammer.

I can help you get up and going with that... it will show you where each and every piece of code comes from.

[Joe788]

Joe, first, I see your missing commas after your n$

pbld, n$, "G05P0", e$

 

And for your "after the last feed line for each operation. I don't know where that is though"

Do you know how to use the post debugger? You NEED to be able to use this for simple post mods... Its like trying to bang in a nail without a hammer.

I can help you get up and going with that... it will show you where each and every piece of code comes from.

 

Keith,

I've never used the post debugger. Let's start there.

[K2csq7]

First you need to enable it.

-Start

-All programs

-Mastercam(Xwhatever)

-McamX control panel applet

 

At the top pick the version your using.

Click "post support" from the tree on the left

enable the post debugger.

 

(not sure if mcam needs a restart at this point or not)

 

Now when you post a program you will see a ladybug in the bottom left corner of the window that pops up.

Click the ladybug and proceed as usual.

The debugger will open.

Hit the play button (green arrow) at the top left.

You will (should) see like 8 windows. The one you want to concentrate on is "NC".

I always maximize that one (I dont know what to do with all the others).

You will see your code being processed under the column titled "nc output"

The column titled "post block" is the one that tells you where the NC output is coming from in the post. (i.e. plinout[1517,22]

The data in the example is coming from the plinout postblock in your post (line 1517 column 22)

 

Let me know if you need more. If your post normally prompts you for questions during the posting process you will have to minimize the debugger and answer the question before the debugging process can proceed.

It isn't 100% as far as EXACTLY where everything is coming from. Sometimes it only leads you to the call for the postblock and you have to trace it back yourself (I have trouble with that sometimes) but you should be able to do 99% of what you are after.

[Joe788]

First you need to enable it.

-Start

-All programs

-Mastercam(Xwhatever)

-McamX control panel applet

 

At the top pick the version your using.

Click "post support" from the tree on the left

enable the post debugger.

 

(not sure if mcam needs a restart at this point or not)

 

Now when you post a program you will see a ladybug in the bottom left corner of the window that pops up.

Click the ladybug and proceed as usual.

The debugger will open.

Hit the play button (green arrow) at the top left.

You will (should) see like 8 windows. The one you want to concentrate on is "NC".

I always maximize that one (I dont know what to do with all the others).

You will see your code being processed under the column titled "nc output"

The column titled "post block" is the one that tells you where the NC output is coming from in the post. (i.e. plinout[1517,22]

The data in the example is coming from the plinout postblock in your post (line 1517 column 22)

 

Let me know if you need more. If your post normally prompts you for questions during the posting process you will have to minimize the debugger and answer the question before the debugging process can proceed.

It isn't 100% as far as EXACTLY where everything is coming from. Sometimes it only leads you to the call for the postblock and you have to trace it back yourself (I have trouble with that sometimes) but you should be able to do 99% of what you are after.

 

OK it's starting to make a little more sense. I'll see if I can figure out where I need to stick it.

[K2csq7]

I'll see if I can figure out where I need to stick it.

Good Luck ...

[Joe788]

Hmmm, I was thinking there'd be a post block for toolchange, a post block for retract, and a post block for "toolpath". Toolchange and retract, yes. The third part, not so much.

[K2csq7]

do you have the mastercam x5 nci & parameter reference guide?

start

programs

mcamx5

documentation

 

if you do take a look at page 147 (the page number on the actual page, not the one adobe says it is)

 

at the bottom of your plinout postblock add this line

 

pbld, n$, "8888888888888888888888888888", *cend$, e$

 

(the "888888888888888" will just make it easy to find.

 

then post your path (without the debugger)

 

Take a look at one of my lathe paths below... notice there is only one place that has the cend varialble as 1 and not 0.... this may be a trigger you can use in your plinout postblock.

 

if mi7$ = 1 & cend$ >0, 
	[
	pbld, n$, "whatever joe wants here", e$
	]

 

 

 

(OP # 6)
N354G00X5.5Z3.H01M00
N356T01H01(TNR = 0.1875)
N358M41C650.S200.M03
N360M8
N362G00X5.8042Z-1.3125
N364Z-2.2346
N366G01X5.9574Z-2.2787E.006
N36899999999999999cend$ 0.
N370G03X5.9629Z-2.2795I-.0055K-.0192
N372X5.9696Z-2.2784I0.K-.02
N374G02X5.9967Z-2.2709I-.0629K.1766
N376X6.0153Z-2.2683I-.0358K.1841
N378X6.0325Z-2.2675I-.0172K.1867
N380G01X6.0512
N38299999999999999cend$ 0.
N384X6.2306Z-2.2626
N38699999999999999cend$ 0.
N388X6.3187Z-2.2234
N39099999999999999cend$ 0.
N392X6.5108Z-2.0805
N39499999999999999cend$ 0.
N396X6.6699Z-2.0113
N39899999999999999cend$ 0.
N400X6.8763Z-1.9663
N40299999999999999cend$ 0.
N404X7.1858Z-1.9267
N40699999999999999cend$ 0.
N408X7.2805Z-1.8904
N41099999999999999cend$ 0.
N412G03X7.2904Z-1.8753I.01K-.0173
N414X7.2905Z-1.8731I.0199K-.0022
N416G01Z-1.8543
N41899999999999999cend$ 0.
N420Z-1.7418
N42299999999999999cend$ 0.
N424G03X7.2867Z-1.7301I.02K0.
N426G01X7.2755Z-1.7145
N42899999999999999cend$ 1.
N430M9
N432G00X5.5
N434Z3.

[Joe788]

do you have the mastercam x5 nci & parameter reference guide?

start

programs

mcamx5

documentation

 

if you do take a look at page 147 (the page number on the actual page, not the one adobe says it is)

 

at the bottom of your plinout postblock add this line

 

pbld, n$, "8888888888888888888888888888", *cend$, e$

 

(the "888888888888888" will just make it easy to find.

 

then post your path (without the debugger)

 

Take a look at one of my lathe paths below... notice there is only one place that has the cend varialble as 1 and not 0.... this may be a trigger you can use in your plinout postblock.

 

 

if mi7$ = 1 & cend$ >0,

[

pbld, n$, "whatever joe wants here", e$

][/code]

 

 

 

 

Hey Keith,

This got me sorta close, except it outputs cend > 1 every time it finishes a contour, whether it be a depth cut, or a different chain. This will actually work just fine, as long as I can put the G05P2 at the START of every depth cut and chain as well. Any idea which variable I should look for and where I should put it for that?

[K2csq7]

Easy fix.Do the same test with cstart$, but put the test line at the top of the plinout postblock.

 

As for doing it "correctly" (i.e. no uncecessary code).

Do you have that parameter reference guide? It lists all kinds of predefined variables. Once you know what they are you can use all you want.

You could pull a parameter value for weather depth cuts are enabled for the toolpath or not (parameter # 15211) then say "if they are on and the current Z value is the same as the toolpaths final depth"... ouput code.

[K2csq7]

 

How's it going Joe? LOL!