527,938 active members*
2,667 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Uncategorised CAM Discussion > Have older CNC that only supports HPGL. What software to use?
Results 1 to 15 of 15
  1. #1
    Registered
    Join Date
    Dec 2010
    Posts
    23

    Have older CNC that only supports HPGL. What software to use?

    Initial point for those who want it short and sweet
    I have an older (1996) CNC that only supports HPGL. The software I am using is Vectric Aspire. The CNC has issues cutting the hpgl that Aspire is outputting. Some things overlap or cut within the same space without moving to the next space. It's probably not Aspire's fault but I want to make sure before I delve into things like retrofitting or other serious steps.

    Is there any software that is specialized in outputting HPGL or one that people prefer to use? Something simple and easy is much preferred but I can make do with any recommendations you post. Free would again be preferred but I would also welcome paid programs as long as it's results are satisfactory.

    Any help would be much appreciated!


    Expanded on for those who are still with me up to this point (Thanks by the way!)
    I am experimenting with the word "Multicam" about 1' long total. It I use a 1D single line font, it cuts great, but if I use the typical 2D fonts with two sides || it cuts out the M then starts the letter U, drives about a foot off the board then back up and continues. No rhyme nor reason for this. I have tried MANY complicated renditions of the letter M and it always works. Italic, Fancy, many lined |||| and they ALL work flawless but when it comes to the next letter (U) it goes haywire. Thanks again!

  2. #2
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Posts
    35095
    I'd contract Vectric and ask them if there is an issue with their HPGL post processor.
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  3. #3
    Registered
    Join Date
    Dec 2010
    Posts
    23
    Quote Originally Posted by ger21 View Post
    I'd contract Vectric and ask them if there is an issue with their HPGL post processor.
    When I last had dialogue with them I made inquiry into their HPGL post processor and was informed it works great, I opted out of expressing my complaints as I then assumed user error, but at the moment, I have run through everything I can think of to check. Final step before starting a ticket with them is to get another HPGL supporting software and see what it does.

    I want to run the same experiments I have (numerous random tests) so I can find out what, if anything at all, is wrong with their post processor. I am also knowledgeable at post-processor editing so I also might just fix theirs and send it back if I can be sure its the software and not my machine.

    Any recommendations would be appreciated!

  4. #4
    Registered
    Join Date
    Sep 2012
    Posts
    1188
    I think that if you can't get Vectric to produce HPGL, you might consider updating the controller before spending money on software that produces code only the smallest fraction of machines understand. I suspect that updating the controller will enhance the capabilities of the machine for about the same money as new software.

  5. #5
    Registered
    Join Date
    Dec 2010
    Posts
    23
    Quote Originally Posted by mmoe View Post
    I think that if you can't get Vectric to produce HPGL, you might consider updating the controller before spending money on software that produces code only the smallest fraction of machines understand. I suspect that updating the controller will enhance the capabilities of the machine for about the same money as new software.
    Was thinking about that as well, but I have no idea how to do this or where TO get it... I also heard upgrading the firmware might work but again, same boat. I did find that I was using the wrong HPGL driver to begin with (Generic HPGL is 2D (PU, PD), Multicam HPGL is 3D (Which I needed all along)) but this was due to the Z Motor driver being physically configured wrong causing the 3D one to not work till I fixed the machine itself. It is still cutting wrong, but at least the code inside the HPGL File makes sense.

    I am assuming it is the machine, but who wants to shell out any amount of money on either software or hardware and not be 100% sure that the money will fix anything.

  6. #6
    Registered
    Join Date
    Mar 2004
    Posts
    391
    The only program I ever came across that had a WIDE, and I mean wide variety of HPGL post variables was/is Signlab. Thats probably because back in the day, there were tons of machines using hpgl.

    About the only help you could get from a Signlab user however is a back and forth attempt to first establish a good test sequence/drawing where specific sized entities in specific locations and subsequently specific cutting order are understood. Then the posted code output could be tested for proper operation and finally, one could attempt to make a test drawing/toolpath that would allow a person to see ALL of the potential variables for that specific control.

    I know what your going thru because I dealt with an MCam MT22 for some time..... it sucks compared to ANY version of G-code, and I would RETROFIT a different control in a heartbeat. Well, not just any control though... I'd definitely use Flashcut !

    Usually, its not the x,y locations of the hpgl, its the many penup, pendown, Rapid rate, cut rate, acceleration subsets that any one particular control COULD use. Each different company did what they felt like, rather than attempt an industry standard for those subsets.

    MultiCam was never one to publish much of that info.... my research led me to Extratech..... the control the Mcams were using at that time.

    ExtraTech Corporation - Motion Control Solutions

    While back in the day, I did attempt to talk to them, I do not recall it going anywhere other than to contact Multicam.

    HPGL was used initially because all Cad programs were intended to "PLOT" to a printer.... wasn't a bad idea necessarily. We would all like to have native G-code output directly from Cad wouldn't we !
    Chris L

  7. #7
    Registered
    Join Date
    Dec 2010
    Posts
    23
    Quote Originally Posted by datac View Post
    The only program I ever came across that had a WIDE, and I mean wide variety of HPGL post variables was/is Signlab. Thats probably because back in the day, there were tons of machines using hpgl.

    About the only help you could get from a Signlab user however is a back and forth attempt to first establish a good test sequence/drawing where specific sized entities in specific locations and subsequently specific cutting order are understood. Then the posted code output could be tested for proper operation and finally, one could attempt to make a test drawing/toolpath that would allow a person to see ALL of the potential variables for that specific control.

    I know what your going thru because I dealt with an MCam MT22 for some time..... it sucks compared to ANY version of G-code, and I would RETROFIT a different control in a heartbeat. Well, not just any control though... I'd definitely use Flashcut !

    Usually, its not the x,y locations of the hpgl, its the many penup, pendown, Rapid rate, cut rate, acceleration subsets that any one particular control COULD use. Each different company did what they felt like, rather than attempt an industry standard for those subsets.

    MultiCam was never one to publish much of that info.... my research led me to Extratech..... the control the Mcams were using at that time.

    ExtraTech Corporation - Motion Control Solutions

    While back in the day, I did attempt to talk to them, I do not recall it going anywhere other than to contact Multicam.

    HPGL was used initially because all Cad programs were intended to "PLOT" to a printer.... wasn't a bad idea necessarily. We would all like to have native G-code output directly from Cad wouldn't we !
    Hmm, from the sound of it, I may want to just use a drop-in retrofit. I heard MachMotion was good, and they are local so I was considering a retrofit from them but they are somewhat expensive and for this machine I really would not like to spend any more large chunks of cash on it. The Flashcut looks like an interesting alternative but with the prices being higher and them being so far away from me, it looks like MachMotion is still my retrofit of choice (For the same cost, MM's come with a pre-configured PC lol).

    As for testing the machine via software I grabbed a trial of Signlab and from looking at it, they removed most of the HPGL outputs in their newer versions. I need to keep digging but from initial look that's what I found. A friend of mine who works on CNC's but is on the other side of the country, said I may be able to flash the firmware to accept GCode, I am skeptical but it certainly would be the cheapest, easiest alternative. I have no idea how to do it, but when he gets back to me I hope that its really something I can do

    The biggest issue, is I found another Multicam on craigslist just the other day online and thought it looked like a good replacement, already configured with GCode, has a tool changer, all the bells and whistles so I was considering selling this one, but I really dont think anyone one there would want this one when it only does HPGL and I can't find a program which outputs well enough to recommend using to a prospective buyer.

    If I can't figure out the while HPGL thing soon enough, I am sure the one on craigslist will be sold in which case I might as well finish retrofitting this one. So many options, so few choices... Brain about to explode xD this whole "Old" CNC Business is beyond my experience or comfort zone. I like new things. LED Monitors, Tablets, i7 processors. When it comes to all of this "has 15 mb of onboard ram" stuff I am totally lost. I just want the thing to run off of Mach 3 on a windows tablet!!!

  8. #8
    Registered
    Join Date
    Mar 2004
    Posts
    391
    I looked at the Multicam post INI files tonight just to see what was in them. They will offer hints as to what the control is "expecting" to see. These are older ones from that era. Note that in the more simple cases, Signlab used JUST the ini file as the complete reference to build a toolpath. However, on harder, perhaps more challenging posts (more likely posts that underlying code would not allow to be created just with the INI), they used a companion .DLL. In this case, an INI called the DLL into play, and the DLL could be developed to do the crazy stuff the INI and base coding could not provide.

    At the way bottom, I'll try to relate what I recall about the INI's. I USED TO know them quite well, but have not needed to know much since I made one for Flashcut and have used it for years the way it is.

    So, this is their 3D one.....

    [version]
    $Revision: 1.5 $
    $Date: 04 Jun 1997 00:40:42 $

    [setup]
    plottername=MultiCam 3D
    page=48000,96000,1016
    ;pagelimit=48100,96100
    notes=
    *****PageX,PageY,Resolution
    cut=0,0,0,0,0,0,1,0,0,0,1,369,372,0,0,0,0,0,0,0,7, 0,0
    tile=0,0,0,0,0,0,0,0
    move1=10,50,200,100,100,0,0,0,0,0,0,0,0,0,0,0,0,0, 0,0,0,0,0,0,0,0,0
    move2=10,50,200,100,100,0,0,0,0,0,0,0,0,0,0,0,0,0, 0,0,0,0,0,0,0,0,0
    move3=10,50,200,100,100,0,0,0,0,0,0,0,0,0,0,0,0,0, 0,0,0,0,0,0,0,0,0
    move4=10,50,200,100,100,0,0,0,0,0,0,0,0,0,0,0,0,0, 0,0,0,0,0,0,0,0,0
    moveLimit1=0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0 ,0,0,0,0,0,0,0
    moveLimit2=0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0 ,0,0,0,0,0,0,0
    MaxVector=999999
    Forced Jog=TRUE
    generic=0
    XYMoveAbs=1
    ArcAbs=1
    ArcSupport=1
    ZMoveAbs=1
    ZMoveUpDn=1
    SendPauses=0
    jog=0

    [MoveControl]
    Variables=4
    V1=Cutting velocity,mm/sec,0,450,SF%d,~
    V2=Plunge velocity,mm/sec,0,100,%d
    V3=Clearance height,.001in,0,10000,~
    V4=Move velocity,mm/sec,1,450,VS%d,~
    V5=Raise velocity,mm/sec,1,100,%d
    V5=Tool number, ,1,8,SP%d

    [Interrogation]
    ;Factors=OF;,500,20,13,%ld,%ld
    ;HardClip=OH;,500,30,13,%*ld,%*ld,%ld,%ld
    ;Digitize=DP;
    ;CurrentPos=OD;DC;,500,30,13,%ld,%ld,%*ld
    PlotterID=OI;,500,50,13,%Fs

    [Generic]
    AbsMove=PA
    RelMove=PR
    MoveUp=PU%.0lf,%.0lf,-200
    MoveDn=PD%.0lf,%.0lf,0
    MoveZ=PU;ZD%.0lf
    Move3d=PD%.0lf,%.0lf,%.0lf
    ;Mode3d=ZZ1
    ;Mode2d=ZZ0
    Tile=
    AbsArc=AA%.0lf,%.0lf,%.2lf
    RelArc=AR%.0lf,%.0lf,%.2lf
    Pause=!OT
    EndJob=ZZ0;SP0
    StartJob=;IN;PU;ZZ1
    Term=;\r\n

    [Tool1]
    ToolInit=
    ToolEnd=

    [Tool2]
    ToolInit=
    ToolEnd=

    [Tool3]
    ToolInit=
    ToolEnd=

    [Tool4]
    ToolInit=
    ToolEnd=!OT
    notes=Head will return to machine origin after job.

    [TOOLS]
    Number Of Tools=3
    Tool 1 Name=Multi-pass
    Tool 1 Type=9
    Tool 2 Name=Single pass
    Tool 2 Type=8
    Tool 3 Name=Braille drill
    Tool 3 Type=6
    Tool 4 Name=Router
    Tool 4 Type=9

    [Resolution]
    ;Low=1
    ;Med=5
    ;High=25
    ;CutResBase=.0254
    ;ArcFitRes=.0254

    [Port Setup]
    ;commset=9600,n,8,1,p
    ;Use DOS Device=1
    TXThreshold=1
    ;TransmitBufSize=10000
    ;ReceiveBufSize=1024
    ;handshaking=0,0,0,0,0,0,0,1,1,17,19,100,900,0,0
    ;ReportError=0xFFFF

    [notes]
    The multicam does not support changing 2d/3d modes in the middle of a job.


    End of the 3d version. Now the plain version:

    [version]
    $Revision: 1.19 $
    $Date: 14 Nov 1996 18:16:04 $

    [setup]
    plottername=MultiCam 22/44/48
    page=48000,96000,1016
    ;pagelimit=48100,96100
    *****PageX,PageY,Resolution
    notes=Depth change will only occur if using Routing or Engraving tool
    cut=0,0,0,0,0,0,1,0,0,0,1,369,372,0,0,0,0,0,0,0,10 ,0,0
    tile=0,0,0,0,0,0,0,0
    move1=10,50,100,100,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0, 0,0,0,0,0,0,0,0
    move2=10,50,100,100,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0, 0,0,0,0,0,0,0,0
    move3=10,50,100,100,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0, 0,0,0,0,0,0,0,0
    move4=10,50,100,100,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0, 0,0,0,0,0,0,0,0
    moveLimit1=0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0 ,0,0,0,0,0,0,0
    moveLimit2=0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0,0 ,0,0,0,0,0,0,0
    MaxVector=999999
    Forced Jog=TRUE
    generic=1
    XYMoveAbs=1
    ArcAbs=1
    ArcSupport=1
    ZMoveAbs=1
    SendPauses=0
    // machine does not jog in real time, it buffers the data
    jog=0

    [MoveControl]
    Variables=4
    V1=Cutting velocity,mm/sec,0,450,SF%d,~
    V2=Plunge velocity,mm/sec,0,100,%d
    V3=Move velocity,mm/sec,1,450,VS%d,~
    V4=Raise velocity,mm/sec,1,100,%d
    V5=Tool number, ,1,8,SP%d

    [Interrogation]
    ;Factors=OF;,500,20,13,%ld,%ld
    ;HardClip=OH;,500,30,13,%*ld,%*ld,%ld,%ld
    Digitize=DP;
    CurrentPos=OD;DC;,500,30,13,%ld,%ld,%*ld
    PlotterID=OI;,500,50,13,%Fs

    [Generic]
    AbsMove=PA
    RelMove=PR
    MoveUp=PU%.0lf,%.0lf
    MoveDn=PD%.0lf,%.0lf
    MoveZ=PU;ZD%.0lf
    Move3d=PD%.0lf,%.0lf,%.0lf
    Mode3d=ZZ1
    Mode2d=ZZ0
    Tile=
    AbsArc=AA%.0lf,%.0lf,%.2lf
    RelArc=AR%.0lf,%.0lf,%.2lf
    Pause=!OT
    EndJob=SP0
    StartJob=;IN;PU;ZZ0
    Term=;\r\n

    [Tool1]
    ToolInit=
    ToolEnd=
    SetPen=SP%d
    notes=Pen number on Multi-Cam will be set to "Tool number" in Color Selection dialog.

    [Tool2]
    ToolInit=
    ToolEnd=

    [Tool3]
    ToolInit=
    ToolEnd=
    ;SetPen=SF%d
    ;notes=Cutting velocity will be set to "Tool number" in the Color Selection dialog. A different velocity can be set for each color.

    [Tool4]
    ToolInit=
    ToolEnd=!OT
    notes=Head will return to machine origin after job.

    [TOOLS]
    Number Of Tools=4
    Tool 1 Name=Pen
    Tool 1 Type=1
    Tool 2 Name=Drill
    Tool 2 Type=7
    Tool 3 Name=Engraver
    Tool 3 Type=8
    Tool 4 Name=Router
    Tool 4 Type=9

    [Resolution]
    ;Low=1
    ;Med=5
    ;High=25
    ;CutResBase=.0254
    ;ArcFitRes=.0254

    [Port Setup]
    ;commset=9600,n,8,1,p
    ;Use DOS Device=1
    TXThreshold=1
    ;TransmitBufSize=10000
    ;ReceiveBufSize=1024
    ;handshaking=0,0,0,0,0,0,0,1,1,17,19,100,900,0,0
    ;ReportError=0xFFFF


    End Plain

    OK, so IIRC, in the case of the following:

    V1=Cutting velocity,mm/sec,0,450,SF%d,~

    V1 = an available variable the control should understand
    "Cutting Velocity" = just a visible explanation of what the "SF" means
    "mm/Sec" = what the number after SF implies
    "0,450" = limitations to keep a user from applying rates the control/machine could not handle (limit)
    "SF" = the beginning of the actual line of code produced to represent in this case: feed rate
    "%d" = the feedrate number as collected from a prior filled out form

    So, "SF35" = feedrate at 35mm per second

    You can gather that the rest in similar strings are... well, similar.

    When you see "%.0lf", its the letters in front that generally dictate the event or axis to be used, and the %.0lf is the LOCATION or related information from the drawing.

    If I can find some time this weekend, I COULD try to pop these drivers into place and create some basic code. Then you could attempt to run it. A guy really needs to see a section of code as it is created because one never knows quite the right SEQUENCE until you have an example. For example, some controls require all of the feedrate, rapid and velocity to be posted right up top and it stays somewhat modal thruout the job. I'd try it now but do not have the dongle with me.

    Well, pick thru that a bit.... see what you see.

    
    Chris L

  9. #9
    Registered
    Join Date
    Mar 2004
    Posts
    391
    >>>Hmm, from the sound of it, I may want to just use a drop-in retrofit. I heard MachMotion was good, and they are local so I was considering a retrofit from them but they are somewhat expensive and for this machine I really would not like to spend any more large chunks of cash on it. The Flashcut looks like an interesting alternative but with the prices being higher and them being so far away from me, it looks like MachMotion is still my retrofit of choice (For the same cost, MM's come with a pre-configured PC lol).

    Where do they start ? Like $2500 ?? Its always up to the retrofitter..... Myself, I'd say you have a WORKING machine essentially... your motors are operational as are the drivers. Myself, I'd opt to open up that cabinet and take a good hard look at the current motor drivers to see if you can stick with them. After all, they ARE working, and even back in those days, MC was running multistep drivers (probably 8 stepping). Then I would just buy Flashcuts Software and sig-gen for about $1200 and tie into those drivers. Then you can have a completely non-buggy, excellent control that runs on practically any windows PC without glitch, without "tuning".... nothing. I've been using $100 laptops for the last few years on my machines... sure beats the space and size required for a desktop. The USB "portability" is fantastic too, as I just grab one of the Flashcut "black boxes" and a laptop and plug it into my small portable CNC plasma machine and am underway in seconds. But to each their own.


    >>>As for testing the machine via software I grabbed a trial of Signlab and from looking at it, they removed most of the HPGL outputs in their newer versions.

    Its more likely that the DEMO just does not show them or have them installed. If you dont mind a sales agent tied around your neck, you certainly could ask them for a demo with multicam drivers installed and I bet they would offer to help if they thought it was worth a sale.

    >> I need to keep digging but from initial look that's what I found. A friend of mine who works on CNC's but is on the other side of the country, said I may be able to flash the firmware to accept GCode, I am skeptical but it certainly would be the cheapest, easiest alternative. I have no idea how to do it, but when he gets back to me I hope that its really something I can do

    That does ring a bell with me. In fact, I think the company I worked for had purchased a G-code option, and it may have been accessible via that "special software" you would install on a Serial port connected PC. It would allow you to look under the hood of the extratech control and play with a few parameters. Almost seems to me that IF you had the G-code "module", you could switch between hpgl and G. I dont think we ever did use it, because we were using signlab, and while it had hpgl drivers for multicam, I dont recall it having g-code drivers for it !

    >>The biggest issue, is I found another Multicam on craigslist just the other day online and thought it looked like a good replacement, already configured with GCode, has a tool changer, all the bells and whistles so I was considering selling this one, but I really dont think anyone one there would want this one when it only does HPGL and I can't find a program which outputs well enough to recommend using to a prospective buyer.

    A prospective buyer certainly can be someone looking or willing to retrofit, but as always, people want a really good deal.

    >>If I can't figure out the while HPGL thing soon enough, I am sure the one on craigslist will be sold in which case I might as well finish retrofitting this one. So many options, so few choices...

    If the machine is solid, has good linear rails and bearings and still runs the way it is, you may as well keep it. You never know what the next one will be like. I know we wore one MT22 to the bone, and I mean the bone.

    >>>Brain about to explode xD this whole "Old" CNC Business is beyond my experience or comfort zone.

    Mach 4 ? It sure will be interesting to see the roll out. They have a lot to prove as its not like prior versions weren't buggy for many users. I've converted more than one machine away from Mach3 for good reason.... just couldn't deal with the quirks. But "explode the old" ?? Well, there are just only so many things that a CNC control needs to do.... I'm curious as to what "new" will really be "new". Just about every trick possible has been exploited by one control or another at this point.

    >> I just want the thing to run off of Mach 3 on a windows tablet!!!

    Well, good luck with that !
    Chris L

  10. #10
    Registered
    Join Date
    Dec 2010
    Posts
    23
    Wow, two amazing Replies. Don't take this short reply as anything less than what it is, an very humble appreciation for all the help being offered. Its just 7am (WAY too early for me) and I have to be at the warehouse to meet an electrician for a unrelated issue and checked my inbox. You have given me a TON of things to look at which I will do for most of the day, needless to say as soon as I do some experiments and research with what has been given to me I will be back with an update! Just dont want to leave no reply while I tinker as that would be rude!

  11. #11
    Registered
    Join Date
    Mar 2004
    Posts
    391
    Here is an actual posted file. This will indicate the SEQUENCE the control is looking for.

    I drew a 4" square with the bottom left corner at 1" x 1", then posted the below with the 2D MCam driver in signlab.


    ;IN;PU;ZZ0;
    SF37,17;
    VS77,88;
    PA;
    PU1016,5080;
    SP0;
    PD5080,5080;
    PD5080,1016;
    PD1016,1016;
    PD1016,5080;
    PU0,0;
    SP0;

    ==========

    Explained version, the way the control must require to see it

    ;IN;PU;ZZ0;
    (In = Start, PU = With PenUp, ZZ0 = 2d Mode)
    (You can see this in "StartJob" inside INI file)

    SF37,17;
    (SF = INI V1 specification)
    (37 = the feedrate I entered in a dialog box)
    (17 = the plunge rate I entered in a dialog)
    (; = Line return(next line))
    >> So the controller wants to see first the feedrate, then plunge rate on the same line separated by the comma <<

    VS77,88;
    (VS = INI V2 specification)
    (77 = the rapid rate I entered in a dialog box)
    (88 = the lift rate I entered in a dialog box)
    (; = Line Return)

    >> Similar requirement for rapid, with the addition of a lift rate <<

    PA;
    (PA = Absolute Move)

    PU1016,5080;
    (PU = PenUp)
    (1016,5080 = Location to run to)

    SP0;
    (SP0 = Tool #zero)

    PD5080,5080; (<< This is where the machine was actually at the 4" x 4" location >>)
    PD5080,1016;
    PD1016,1016; (<< This is where the machine was actually at the 1" x 1" location >>)
    PD1016,5080;
    (PD = PenDown and to locations shown)

    PU0,0;
    (PU = PenUp to locations shown... 0,0)

    SP0;
    (SP0 = End Job (must be same as tool change... perhaps go to home position)

    Note the reference to 1016. The fact that the post driver indicated 1016 would tell me the machines default is the common 1016 "units" setting, which usually correlates to 1016 steps or units per inch of travel. I recall sometimes setting a machines Units to 1000 (when possible), that way you had nice
    round numbers to look at in the code... IE: 1000 = 1", 4000 = 4" Etc.

    Well, thats a start I guess. If you want to replicate the events, you certainly CAN do this with plain old Corel Draw (as long as its not their cutback versions that do not have hpgl export). Export to hpgl "file" in corel with units set to 1016. Corel will put in the PenUp and PenDown along with positioning in the file. You just need to ADD IN the other information like the feeds and speeds in the locations shown above, then do a simple file copy (look up the old DOS copy command) to the machine port. I dont recall that being any harder than going to a command line and putting in something like:

    copy path/filename.txt lpt1 (or Com1, etc)

    With that, the file would be loaded in the control, waiting for you to hit start on the control after setting your program zero location.

    I will need to get a bit more "creative" to give you a toolpath with 3d hpgl in it as I really do not have a 3d version of Signlab. I can however tell individual nodes to be at varying Z heights and it should create something for me.... we'll see.

    Now when you are all done learning about hpgl and how it CAN be applied to CNC (when desperate measures are demanded), you will need to go find a doctor to look at that bright red swollen forehead. Frankly, you will find yourself banging your head against the wall over and over, screaming "this can't be that hard, dammit!". You've been warned ! :-)

    To which end you will eventually convert that machine to a G-code control... Ahem... like Flashcut, then use an elegant, inexpensive yet powerful program like V-Carve to create easy to understand code that will run on your easy to understand control and float through this like a butterfly. LOL !

    Seriously, hpgl works for many simple devices like pen and vinyl plotters, perhaps simple drag engravers..... but not for more capable machines. I been there, I done that.
    Chris L

  12. #12
    Registered
    Join Date
    Dec 2010
    Posts
    23
    Update: I built a HPGL 3D post processor that works with aspire witch fixed the overlapping models, The problem I am having now is
    that at a random repeatable (per file) point the head drives to max X or Y then back to the model and continues for a bit Then will do it again.
    the program will finish but has multiple lines across the table/board. The issue might be with the cnc and not the code.

  13. #13
    Registered
    Join Date
    Dec 2010
    Posts
    23
    Working: I Finally got it working, turns out the Dnc program I was using "WDNC95" was bad.
    I am now using MultiCam Suite 4 Download Link Below, Its all setup and running I am using Vectric Aspire with A custom Post Processor for 3D HPGL
    Thanks to Everyone who helped me.


    MultiCam Suite 4 And other cnc software.
    MultiCam Southeast | CNC Plasma, CNC Laser, CNC Waterjet, CNC Router Bits


    This is My Post Processor I change it to Inches from MM and modified the Footer
    "MultiCam_Plt_INCH 3D.pp"
    Code:
    POST_NAME = "MultiCam Plt 3D (inch)  (*.plt)"
    
    FILE_EXTENSION = "plt"
    
    UNITS = "INCHES"
    
    RAPID_PLUNGE_TO_STARTZ = NO
    
    +================================================
    +                                                
    +    Formating for variables                     
    +                                                
    +================================================
    
    VAR FEED_RATE = [F|A||1.0|0.0166]
    VAR X_POSITION = [X|A||1.0|1016]
    VAR Y_POSITION = [Y|A||1.0|1016]
    VAR Z_POSITION = [Z|A||1.0|-1016]
    VAR X_HOME_POSITION = [XH|A||1.0|1016]
    VAR Y_HOME_POSITION = [YH|A||1.0|1016]
    VAR Z_HOME_POSITION = [ZH|A||1.0|-1016]
    
    +================================================
    +                                                
    +    Block definitions for toolpath output       
    +                                                
    +================================================
    
    +---------------------------------------------------
    +  Commands output at the start of the file
    +---------------------------------------------------
    
    begin HEADER
    "IN;PA;ZZ1;SP1;"
    
    
    +---------------------------------------------------
    +  Commands output when feed rate changes
    +---------------------------------------------------
    
    begin FEED_RATE_CHANGE
    "SF[F];"
    
    +---------------------------------------------------
    +  Commands output for rapid moves 
    +---------------------------------------------------
    
    begin RAPID_MOVE
    "PU[X],[Y],[Z];"
    
    +---------------------------------------------------
    +  Commands output for the first feed rate move
    +---------------------------------------------------
    
    begin FIRST_FEED_MOVE
    "PD[X],[Y],[Z];"
    
    +---------------------------------------------------
    +  Commands output for feed rate moves
    +---------------------------------------------------
    
    begin FEED_MOVE
    "PA[X],[Y],[Z];"
    
    +---------------------------------------------------
    +  Commands output at the end of the file
    +---------------------------------------------------
    
    begin FOOTER
    "PA0,0,[Z];"
    "ZZ0;SP0"

  14. #14
    Member
    Join Date
    Jul 2017
    Posts
    197

    Re: Have older CNC that only supports HPGL. What software to use?

    Im looking for a hpgl 3d post processor that will work with new hermes v3400
    Anyone familiar?

  15. #15
    Member
    Join Date
    Jul 2017
    Posts
    197

    Re: Have older CNC that only supports HPGL. What software to use?

    Do anyone know what this command means in a output engraver code hpgl

    !PZ0,500

Similar Threads

  1. Buying older/used versions of software/rhinocam - possible? tips?
    By danielcoyle in forum Uncategorised CAM Discussion
    Replies: 10
    Last Post: 01-24-2014, 09:45 AM
  2. Software to work with older GSI Lumonics?
    By ralph@nes in forum General Laser Engraving / Cutting Machine Discussion
    Replies: 1
    Last Post: 01-21-2014, 03:05 PM
  3. Buying and Using Older CAD/CAM Software
    By bothunter in forum Uncategorised CAM Discussion
    Replies: 0
    Last Post: 02-12-2008, 05:59 AM
  4. HPGL help me!
    By vacpress in forum Printing, Scanners, Vinyl cutting and Plotters
    Replies: 2
    Last Post: 01-09-2006, 10:49 AM
  5. Software for an older machine?
    By CamWest in forum Commercial CNC Wood Routers
    Replies: 1
    Last Post: 07-08-2005, 03:02 PM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •