postprosser not working for me

[nccuctoms]

hay there i love sheetcam so far how ever i cant really use it so well i have an older hpgl style router the hpgl 3d post seems to work but the
Z hights are all wrong and the feed rate is not being sent trough and i cant seem to find the ONsetfeedrate part of the post

i have a post for desk proto that is so simple but works amasingly

all it has is for 3d moves=
ZM x,y,z;
set feedrate =
VS#;
rapids = PU x,y,z

no AA comarnds used and works like a charm
the AA in the HPGL 3D post work ok to but for some reson if i program
something to say cut at 3mm it will only cut at about 1.5 mm

hpgl scale is good ive cut a shape and mesured it and its perfect

could you please re work the post for me i have spent meny hours trying to do it but i am afraid i dont quite understand how sheetcam posts are worked
i allso need to remove the tool change from the post so regardless of the tool used in sheet cam the post still reeds SP2 an not related to the tool used in sheetcam
your help would be verry much apresheted

thank you heaps

[nccuctoms]

heres is a good post from my desk proto

[nccuctoms]

heres is a good post from my desk proto

[nccuctoms]

here is the hpgl 3d plot language my router uses hopefully one of you gurus can help me to get sheet cam to make it

SP select pen (tool select ) i have not tool changer so i need it to reed SP2 all the time

syntax
SP;
SP toolnumber;
SP toolnumber,spindlespees;

syntax
VS, velocity select (set feed rate )

VSvelocity; number = feed rate in mm/sec


PA, plot absolute (sets absolute progmaming)

syntax
PAxpos,ypos

if pen up rapid feed used
if pen down profiling feedrate used

PU pen up (pen up move )
syntax
PUxpos,ypos; (move to pos with pen up)
PU ( rase tool to safe Z)

PD pen down ( pen down move )

syntax
PDxpos,ypos;
(moves with tool down an feed set by VS comarnd )

AA absolute arc
syntax
(AA darws an arc starting an current location)
AAxcenter,ycenter,sweepangle ;
(sweep angle is the angle in degreese trough wich the
arc is darwn a positive angle darws counter clockwise )
AA10000,10000,360 (plot a circle with center x100y100)

ZM 3 dimensional move

syntax
ZMxpos,ypos,zdepth;
(Auto pen down with ZM move will move from current to new pos with VS feed rate an !VZ plunge rate for z axis

!vz z axis feed rate
syntax
!vzvelocity;
!vz10.3;(sets z velocity to 10.3mm/sec)

!PZ set plunge depth
syntax
!PZplunge-depth; (sets only pen down depth)
!PZplunge-depth,safe-hight; (sets plunge depth and safe hight)

!PZ-500,300; (set plunge depth to 5mm and safe hight to 3mm)
!PZ-1000; (set plunge to 10mm)

MG send message to operator screen
syntax
MGmesage;(message will be desplayed on the operator screen)

NR not ready (M00 stop press start to continue)
syntax
NR; ( macheine will stop untill start button is pressed )

all examples in the code above uses 100 hpgl steps per mm
and programing is absolute

this is standard hpgl 2 language or MIMAKI ME-500

ANY HELP GETTIN SHEETCAM TO MAKE THIS POST WOULD BE GREATLY APRESHETED

CURRANTLY I AM MAKING ALL MY TOOL PARTHS IN CAD AND IT TAKES ME A COUPLE OF HOURS TO PROGRAM EACH JOB WICH IS USED ONLY ONCE

[nccuctoms]

this is the post i was tryin to use

[nccuctoms]

ok les may have the bualk of it sorted got the feeds to work and added code to set z

it is probaly 5x to often but it works none the less

i started with the stock hpgl post and added the !PZ to set plunge
each line

i have been working al day on the post trying it and editing it and re trying on the router

i added in to the oninit

scale = 100
post.Text("IN;PA;PU;\n")
post.Text("VS")
post.Text ( feedRate * scale, "0" ) lastinst = 0
arcscale = -57.2957795130
bigArcs = 1 --stitch arc segments together
minArcSize = 0.05 --arcs smaller than this are converted to moves

note the feedrate is still not being brought in to the program it is allways 0

the post works well but i just have to set the feed once the file is loaded in to the cnc

i changed the tool call to allways reed sp2
think i still need is to add the a stop so i can change the tool when needed

if you could have a look at the post andsee if it is fine and see if you can spot any
issues or a beta way to do the feedrate
or plunge rate

i allso added a set safez in to the tool change so its in the top of the program

any way here is the 2 files the post and the output file

end

[Les Newell]

Sorry it has taken me so long to reply to this thread. Give the attached post a try. It uses ZM 3-axis moves for all moves except arcs.

[nccuctoms]

the post is awsome had to add a ";" to the check feeds and swiched the rapids back to a normal PU endxX endY

the tool change is perfect

one thing that dont work wick is really stupid of this plot language
is when useing a ZM endX endY endZ the -prefix needs to be removed

its stupid becouse with an !PZ -100,400; this sets plunge to -1mm
but in the cace of ZM 100,100,-100 this moves to x100y100 and +1mm
above the top of the work

when the ZM call has a z value it will set the plunge for all other moves
wich is programing awsomely becouse befour each AA it post a ZM with the z value

so in short form is there a way for us to remove the - from the Z feild when posting ZM i allso havent tryed the post for a drill cycle

i will attach a copy of the post you sent me with my tweeks so you can see how it will work

changeing the rapids to PU removes any Z from it and it pen ups to the
!PZ in the header of the program wich is the safez from sheet cam

[nccuctoms]

Sorry it has taken me so long to reply to this thread. Give the attached post a try. It uses ZM 3-axis moves for all moves except arcs.

and no worrys about the time taken to reply it gave me a beter understanding of the way the post works az i spent a good amount of time playin with it trying to figure out how it ticks wich is quite fun tryin out bits of code and then re posting hopeing it works then trying to figure why it dosant i think you do a awsome job with sheetcam its probly the only cam program with this leval of support and its allmost the only one that still supports hpgl other cam programs will tell you na mate your macheine is to old you need to retro fit a new control to it

to wich i strongly disagree my controler is great it has it has 8 buttons and joystick its simple and easy to use

you load the program from the panal set the oragen set the z and hit the run button

[Les Newell]

It is easy to reverse the Z axis:

Code: Select all

post.Number ( -endZ * scale, "0")

I used ZM for rapids because sometimes SheetCam issues rapid moves to heights other than the safe Z. For instance when peck drilling you may want to only retract a small amount. Do you think using ZM moves with a high feed rate would work? It would be easy enough to tweak the post to do that.

[nccuctoms]

yea it would work just as well it just seemed simpler to use the pu becouse i know i could make it work and to check the ouput it breaks it up a bit so i can see the rapids in the file but my other program uses zm to rapid also so i will change that z- and give it a try useing zm for rapids an maybe ill add an extra space or like so i can reed the file more easly

i was haveing anothr play today and changed the zm on move to PD with an !pz and ran it wich worked well too

[Les Newell]

The problem with PD is that you won't be able to use ramp cutting. Ramping the cut start is much easier on the cutter and the machine. It can also prevent burning at the cut start.

[Martinizhr]

Hello,

I am having the same problem. I have tried downloading the post-processor files, but they are no longer available. Can someone repost the files?

Big thanks in advance.

[Les Newell]

Unfortunately quite a few download links broke when I upgraded to PHPBB3 some years ago back. It took a bit of hunting though backups but I think this may be the file you want.

[Martinizhr]

Thank you for your fast reply.
I will try it out. Hopefully, it works as I do not know how to make my own driver. xD