B axis in Machine definition and post?

[Uhrenholt]

H there

I have made some changes in the old post so my Maho 800 can run as an HMC. The next thing is to do some B axis movement, if possible. Turn 90degree drill a hole, turn 90degree and mill pocket. The control doesn't support G54 - G59 offsets, so this has to be done from the middle of the rotating axis.

Do this need to be in the .pst file, or can this be made in mastercam just to rotate the B axis? I don´t need all 4 axis to move a the same time.

Are there any good training online about planes and indexing, or some books just need to have if I can figure this out.

Or do anyone know where to get a post for an Maho 800 C with Phillips 432 control to a fair price, or do someone have an post they are willing to share?

I can upload the post that I have tomorrow, but it is almost the same as the one in a former thread of mine. I'm away for a festival today, so cant upload before tomorrow when I come home.

Cheers, Daniel

Similar Threads:

• New Machine Build- need help - understanding machine definition and setting it for my machine
• New Product- Super Definition Plasma Cutting Machine Upgrades High Definition Plasma Cutting
• Need Help!- Custom Machine Process Definition / DATRON MCR Post
• Build Thread- Machine Definition
• wrong machine definition , post processor issue ??

[Superman]

. The next thing is to do some B axis movement, if possible. Turn 90degree drill a hole, turn 90degree and mill pocket. The control doesn't support G54 - G59 offsets, so this has to be done from the middle of the rotating axis.

Do this need to be in the .pst file, or can this be made in mastercam just to rotate the B axis? I don´t need all 4 axis to move a the same time.

Or do anyone know where to get a post for an Maho 800 C with Phillips 432 control to a fair price, or do someone have an post they are willing to share?

I can upload the post that I have tomorrow, but it is almost the same as the one in a former thread of mine.

Daniel

If your post IS a modification of the post that I worked on.......bad news.... it is a 3 axis post only, no rotary axes are in it
- another post is needed...look for a MAHO_4 axis.pst, a 4axis MMD file & CONTROL

fingers crossed for you
( if your Mastercam is legit & you are on maintenance, try obtaining the files from your reseller. They should have a Generic file(s) that you can customise yourself...not sure on cost )

[Uhrenholt]

Daniel

If your post IS a modification of the post that I worked on.......bad news.... it is a 3 axis post only, no rotary axes are in it
- another post is needed...look for a MAHO_4 axis.pst, a 4axis MMD file & CONTROL

fingers crossed for you
( if your Mastercam is legit & you are on maintenance, try obtaining the files from your reseller. They should have a Generic file(s) that you can customise yourself...not sure on cost )

I got an generic file that I just got this morning:-) now I have to edit the post so it works with my needs:-) maybe there will be some questions along the way, but it is much more up to date than the post I got with the machine.

Cheers, Daniel

[Uhrenholt]

Hi I have some problems with the new post.

I have made the header and end of program as I want it, but I have a problem with figuring out how to make a M66 when the tool number is greater than 30, as the machine only has 30 tools in the machine, so have to put tools in it with an M66.

I tried to use the code that superman made in the new post, but without luck.

I put maho and mach under formulas and I have copied the code from the old post to ptlchg$, but it doesn't work. And I have no clue why.

There are still some problems with empty lines when generating G1 G2 G3. but I'm trying to figure that out:-)


I haven't tried to post anything to the machine yet, as I had an little accident with my fingers yesterday, with an grinder machine, so cant do anything with oil for a week!

Cheers, Daniel

[Superman]

Hi I have some problems with the new post.

I have made the header and end of program as I want it, but I have a problem with figuring out how to make a M66 when the tool number is greater than 30, as the machine only has 30 tools in the machine, so have to put tools in it with an M66.


I put maho and mach under formulas and I have copied the code from the old post to ptlchg$, but it doesn't work. And I have no clue why.

1st toolchange is in psof, the remaining toolchanges uses ptlchg$, ......... an op using the same tool is ptlchg0$

this is what you need at the 2 places, it is an auto-decision on what value is held by "mach"

           n$, "G17", ss$, t$, [ if t$ > mach, "M66", else, "M6" ], e$

your 2 lines for the retract in ptlchg$ could be changed to this

         n$, psg00, [ if prv_t$ > mach, "Z100" ] , "M5", e$

PS....Grinders bite

Look at the bottom of the pst I did for you ... all the [CTRL_MILL|DEFAULT] to the [CTRL_TEXT_END]
- copy & paste it to this new post to get the drill cycle text to be the same....one section should have the same name as this new cnc_machine ie [CTRL_MILL|MPMAHOXY]

[Uhrenholt]

some of it seems to work:-)

I have little problem getting the spindle speed working in ptlchg$.

It goes as follows:

ptlchg$ # Tool change
if coolant$ = 0, n$, smcool,e$
n$, psg00, [ if prv_t$ > mach, "Z100" ] , "M5", e$
n$, "G17", ss$, t$, [ if t$ > mach, "M66", else, "M6" ], e$
# n$, ss$, t$, "M06",e$
n$, "M03",e$
pcan
pcan1, n$, strcantext, e$
pcan2
n$, mr2$, mr1$,e$
if coolant$ <> 0, n$, smcool,e$
prv_x$ = xh$
prv_y$ = yh$

Probably no need for the G17...

Tool change is right, but there are no spindle speed generated.

N1880 M9
N1890 G0 Z100 M5
N1900 G17 T2 M6
N1910 M03

Grinders bite you say, I almost lost a finger! So no going to the shop until my finger is somehow fine again... Du not stress when you are in a hurry, bench grinders and sheet metal can REALLY mess you up!

"EDIT"

I just have on more Q

What is pcan, pcan1 and pcan2?

[Uhrenholt]

I got it working:-)

Probably worked yesterday also, but had to restart mastercam before changes occur.

But it goes Z150 when changing with M6, doesn't really matter...

Trying to fix the empty line numbers now, but I really have a hard time seeing where it is.

Any good ideas where to search?

Edit

Some of the empty lines had something to do with pcan and pcan1, I deleted them and the post looks much better now:-)

Still have a problem with G2 and G3.

Cheers, Daniel

[Superman]

pcan is associated with the "Canned text" section....probably no effect for you

spindle speed
try changing the ss$ to *ss$ in psof & ptlchg$
- the asterisk is to force that into the NC file.....best to have it forced at the toolchanges ( & at the ptlchg0$ only if it alters )

"it goes Z150", your posted segment shows Z100 ?

Just had a flash,
- the "n$, psg00, [ if prv_t$ > mach, "Z100" ] , "M5", e$" needs altering....to consider current tool AND incoming tool....it need the "extra lift" to allow the manual toolchange
- change that line to be "n$, psg00, [ if prv_t$ > mach | t$ > mach, "Z100" ] , "M5", e$" ..... that character is an "OR"

[Uhrenholt]

Thanks superman it is working now:-)

The canned text did something, i got rid of some empty lines when deleting them.

But I cant figure out what is forcing the empty line, I don't have any pbld n$ or e$ doing anything as I can see, so it may be something similar to the problem I had with the old post.

I have uploaded the Post with my reply, so if you can take a look at it I will be very grateful.

I did go to the workshop today anyway, so is meddling with the machine now:-)

Cheers, Daniel

[Uhrenholt]

Could it be sscomp under # Cutter compensation string select that makes this line? there is only "" as text.

pcirm # Circular interpolation
n$, sccomp, e$
if plane$ = 0,pcan1,n$,sgplane,sgcode,*x$,*y$,*xc$,*yc$,z$,pfr ,strcantext, e$
if plane$ = 1,pcan1,n$,sgplane,sgcode,x$,*y$,*z$,*yc$,*zc$,pfr ,strcantext, e$
if plane$ = 2,pcan1,n$,sgplane,sgcode,*x$,y$,*z$,*xc$,*zc$,pfr ,strcantext, e$

[Superman]

Could it be sscomp under # Cutter compensation string select that makes this line? there is only "" as text.

I'd be careful with what you remove, the "" is the default if nothing is currently stored, You have to consider the possibility of something having stored info that needs to be output later....I'd say "canned text" won't be used


To see if it is that line, put an asterisk (*) to force the postblock out to the NC file
- you may be correct , as it is occurring before any arc

hint....to find if you are at the correct line, put something like "HERE", ,save then post some code.....this is called hardcoding, forcing specific text into the NC file, for this purpose, use code that would make the machine throw up an error ( if accidently run )

pcirm      # Circular interpolation
           #n$, *sccomp, e$
           n$, *sccomp, "HERE", e$    
           if plane$ = 0,pcan1,n$,sgplane,sgcode,*x$,*y$,*xc$,*yc$,z$,pfr,strcantext, e$
           if plane$ = 1,pcan1,n$,sgplane,sgcode,x$,*y$,*z$,*yc$,*zc$,pfr,strcantext, e$
           if plane$ = 2,pcan1,n$,sgplane,sgcode,*x$,y$,*z$,*xc$,*zc$,pfr,strcantext, e$

[Uhrenholt]

It was that line of code, deleted it and now it is just fine:-)

The only issue I have now is that it puts too many digits out when making G1, G2 and G3, But I have to change something in the control definition I think, There are a tolerance that is 0.0001. But I have done that and it still spits out 0.0001 instead of 0.001 that the machine can use. too many digits and I get a fault. I will try tomorrow again and see if it helps when I reboot the computer. My head is tired now after meddling with that post for the last days, better grab a beer and enjoy the sun now:-)

Thanks for the help, now I just have to figure out how to make the planes for 4 axis machining, so I can see if the Post generates the code for the B axis:-)

Cheers, Daniel

EDIT

Problem solved

The thing is if I draw an arc, it has to be within 0.001 mm, one digit more makes my problem:-)

now to the next thing, making the axis in the machine configuration match the machine. If that is necessary if it has to work with the post for 4 axis tasks? It is A generic file I have so A B axis has t be deleted and B has to be tilted to the right position, right?

This is a whole new world t me,I have been milling with 3 axis milling machine for 10 years now, putting one more on just makes it all a little harder, but a lot more fun:-)

[Uhrenholt]

Hi again folks

Just as i thought I had it, a new problem occurred. This is a bit hard to explain i just one line, so a little code:

N210 G17 S3500 T2 M6
N220 M03
N230 B0. F0.
N240 G0 X-75. Y10. Z999.999
N250 G0 Z25.
N260 G0 Z10.

As you can see Z is going 999.999, much more than the machine can do:-) I get this fault when post processing.

PST LINE (613) - Label has not been defined[5]
PST LINE (613) - Label was expected but was not found[8], Illegal character(s) encountered
PST LINE (260) - The math calculation/formula has an error
PST LINE (261) - The math calculation/formula has an error

The code at line 613 goes:

plinm # Linear line movement - at feedrate
pcan
if prv_cc$ <> cc$, pcan1, n$, *sgcode, x$, y$, z$, pfr, strcantext, e$, n$, sccomp
if prv_cc$ = cc$, pcan1, n$, sccomp, sgcode, x$, y$, z$, pfr, strcantext, e$
pcan2

How do I define plinm? as it makes my fault with z going 999.999?

the two other faults are:

N260 omitrefht : no$ # Don't use reference height on first non-canned Z move
N261 eqmax$ : 9999 # Max. sequence no.

Have no Idea what the do, but it is a no for omitrefht

Any ideas?

Cheers, Daniel

[Superman]

N210 G17 S3500 T2 M6
N220 M03
N230 B0. F0.
N240 G0 X-75. Y10. Z999.999
N250 G0 Z25.
N260 G0 Z10.

As you can see Z is going 999.999, much more than the machine can do:-) I get this fault when post processing.

that is an initial ( or starting value)
- are you really confident, in your ability to edit a post ?

pinit      # Initialize Vars
           prv_fr$ = 999.999
           prv_frplunge$ = 999.999

           prv_x$ = 999.999
           prv_z$ = 999.999

PST LINE (613) - Label has not been defined[5]
PST LINE (613) - Label was expected but was not found[8], Illegal character(s) encountered
PST LINE (260) - The math calculation/formula has an error
PST LINE (261) - The math calculation/formula has an error

The code at line 613 goes:

plinm # Linear line movement - at feedrate
pcan
if prv_cc$ <> cc$, pcan1, n$, *sgcode, x$, y$, z$, pfr, strcantext, e$, n$, sccomp <---- no e$.....why ?? (find the reason before just plonking it in , or commenting it out )
if prv_cc$ = cc$, pcan1, n$, sccomp, sgcode, x$, y$, z$, pfr, strcantext, e$
pcan2

How do I define plinm? as it makes my fault with z going 999.999?

plinm is NOT at fault, it is something on line 613......you've put up 5 lines, which is line #613
.....the 1st "if" line is strange, there is a end of line (e$) then more info without an e$

the two other faults are:
N260 omitrefht : no$ # Don't use reference height on first non-canned Z move
N261 eqmax$ : 9999 # Max. sequence no. .......... look at the original pst file.....you've lost the "s" at the beginning....no wonder it gave back an error

Have no Idea what the do, but it is a no for omitrefht
.....could be a result of removing pcan callups.......were these errors there before your pcan edits ???

my other concern with this post is the reason behind the need of M03 on lines, same goes for addresses that are modal ie G0
- this 4 axis post seems to have been modified by a novice ( before you )

Have you cut & paste lines from one post to another ?

[Uhrenholt]

I started from scratch and got it working:-)

As you asked, no I am not confident about this, but if I want to learn it I have to start somewhere. As an educated toolmaker, I taught myself to build Tesla coils and other electronic, making PCBs, soldering, working with high power semiconductors, and have done some rather groundbreaking stuff thru the years with an friend of mine. Stopped doing electronics 4 years ago, as my former job at a university took all of my time, as I was designing and building UAVs and satellites with research groups.

I still have to edit some with the canned drill cycles, as I have to make a chip break cycle in mastercam to get an G84 tapping cycle, Ill have that done by the weekend

Any good books or reading about post processors on the net?

Cheers, Daniel

[Uhrenholt]

Hi,

I need to make new drill cycles, as the ones that are in the post is rather messy. running G79, and it looks bad. Is there an Easy way to do this? I need to make a new drill varible formats, and new cycles. someone Have made some changes I can see, but it doesent add up, it doesent work.

There are still a problem about the post spitting out 0.0001 instead of 0.001, and I cant get my head about it. Any suggestions? maybe the post is for inch?

I have added the pst again.

Maybe I should find someone who will do this for me... I would like to do it myself, but it is one step forward and two steps back at the moment....

Cheers, Daniel