Share
Results 1 to 18 of 18

Thread: New diy cnc machine pp50 with thc

  1. Default New diy cnc machine pp50 with thc

    I just finished a 4 foot by 4 foot cnc table. It worked well except that the torch tip would touch and drag and last only a very short time then mess up the project.
    I bought a proma thc and mounted it to the pp50 ,and it recorded around 54v ach voltage raw volts,so the low volts made the torch lift and stop cut.
    I am using sheetcam with mach3 and bob is a tb6560 4 axis.
    I read that the raw arc voltage should be 88v at 20amps and about 100v at 50 amps
    I was running at 30 amps and the reading on the thc readout was around 54v.
    My lead from the pp50 it about 3 to 4 feet long in shielded cable. would this length cause that big voltage drop....(proma instructions said to keep this lead short)
    This has been a fun learning project to purchase parts on ebay from all over the world, build and wire the machine .learn 3 software programs,etc.
    I am 59 and trying something new for a little hobby.
    I hope that this thc problem will be the end of my challenges for a while.
    I don't mind a few challenges but it will be fun to do a few projects now.
    thanks for any help
    Wayne

  2. #2

    Default

    There are a few questions do you have the THC turned on in Mach3 this is on the front page of Mach 3 see picture. Next do you have THC option turn off in ports and pins. Having this on caused my problems similar to what you are having. Another thing you need to run the plasma unit to the spects of the torch tip if you have a 40 amp tip run it at 40 if you have a 60 tip then run 60. This will have a big effect on the raw volts at the tip. You did not say if you are using the pierce function or a delay before cutting. You should start at about .160” light the torch delay .4 and drop to .060” for cutting. At this point the THC will check the raw volts and adjust the height and follow the metal surface. You will need to make test cuts to find what works with your setup.
    Do you have the THC setup in the SheetCam post-process so it can tell mach how to operate the Z up-down command.
    Do you have afloating head setup on your Y axis to touch the metal to zero the Z location?
    Have you checked to see if the THC signals are getting to Mach and are correct? run the Proma test and watch in the diagnostic page of Mach.
    http://www.youtube.com/watch?v=aoXIRMLx8Sg Mine before I cleaned up the settings.
    I went through the same things built my own table learned the software and I'm 70 Oh what fun it is to see the table work.
    Attached Thumbnails Attached Thumbnails Click image for larger version. 

Name:	THC options.jpg 
Views:	2066 
Size:	36.8 KB 
ID:	11632   Click image for larger version. 

Name:	THC front panel.jpg 
Views:	732 
Size:	26.3 KB 
ID:	11631   Click image for larger version. 

Name:	dignostic page.jpg 
Views:	1749 
Size:	62.2 KB 
ID:	11633  
    Last edited by acourtjester; 01-01-2014 at 04:12 PM.

    Everlast PM256
    Millermatic 180
    Hypertherm PowerMax 65 with machine torch
    Longevity Force Cut 80I
    DIY CNC table for plasma/routing
    13" metal lathe
    Small Mill
    ect, ect.

  3. Default

    I have thc option on in ports and pins.
    I have thc in mach3 screen off no green light. when I had it on the torch would not move and cut.
    I was running at 30 amps maybe I will try 40 plus amps
    I have pierce and delayand cut height very close to your specs.
    In sheet cam I am just using mach3 with pause no thc . Iam not sure what one would be best for me.
    proma test moved the torch head up and down. I will have to check it against the diagnostic page in mach3
    thanks I maybe a couple days as we have family for new years here and sons car to fix in the shop and 2 grand children to play with
    catch you later
    Wayne

  4. #4

    Default

    Ok let me tell you this I use a modified post processor so the Mach knows to look for the THC. If I want to do a dry run (no torch on) I leave the green THC light out and the table will drive around and go through all the moving about the metal just does not light the torch. I do this to insure I am not going off the edge somewhere. I make sure my G-code has a return to the starting position at the end of cutting. G0Y0.0X0.0 as the next to last line you can edit the g-code in Mach after you load it just save and exit the edit after you add this line. If you have the green light on and try this it will move to the first cut location find the metal surface then go to pierce height and try to cut the THC does not send arc ok and mach stops there.

    In sheet cam under options select machine and then edit post processor I did this to Mach 3 plasma and scrolled down to (function OnPenDown() and clear out whats in there and copy and paste this in its place. Then rename it like mach 3 plasma (your name) and save and use this for the post processor to make the g-code.

    function OnPenDown()
    if (preheat > 0.001) then
    post.ModalText (" G00")
    post.ModalNumber (" Z", cutHeight * scale, "0.0000")
    post.Text ("\n G04 P")
    post.Number (preheat,"0.###")
    post.Eol()
    end
    post.ModalText (" G00")
    post.ModalText ("\n G90F30\n")
    post.ModalText (" G28.1 Z0.50\n")
    post.ModalText (" G92 Z0\n")
    post.ModalText (" G0 z0.25\n")
    post.Text (" Z")
    post.Number (pierceHeight * scale, "0.0000")
    post.Text ("\n M03\n")
    if (pierceDelay > 0.001) then
    post.Text (" G04 P")
    post.Number (pierceDelay,"0.###")
    post.Eol()
    end
    end

    This will make Mach 3 do the touch the metal surface for each new cut location

    Everlast PM256
    Millermatic 180
    Hypertherm PowerMax 65 with machine torch
    Longevity Force Cut 80I
    DIY CNC table for plasma/routing
    13" metal lathe
    Small Mill
    ect, ect.

  5. Default

    With the code added do you have to have a floating head with micro switch?
    how does the z axis know when it touches the steel?
    My machine doesent have the micro switch on z
    also your go to x o and y o did not accept on my sheetcam is there a type error on that line?

  6. #6
    Join Date
    May 2012
    Location
    Disneyland
    Posts
    2,661

    Default

    Quote Originally Posted by waynagen View Post
    also your go to x o and y o did not accept on my sheetcam is there a type error on that line?
    Be sure you are not mixing up the number zero with the letter O. (0O) It helps to use a font where the zeros have a slash through them if you have trouble.
    G codes are numbers and X and Y positions are also numbers. It helps to have decimal points, even though most controls do not require them.
    Also you can have leading zeros on single digit G codes, even though most controls don't need them. It will make the code a little more readable.

    For example:
    G00
    G01
    G02
    etc.

    Spaces are also ignored, but can make your code a lot easier to read. These lines all do the same thing but are written differently.
    G0X0Y0
    G00X0.Y0.
    G00 X0.0 Y0.0

    You might want to get a good overview of G-code, even if SheetCAM is creating most of the code for you. That way you will better understand what is going on and be able to make tweaks to the code when something isn't quite right, without having to find a way to tell SheetCAM about it and regenerate the code.
    In this case G0 (or G00) is a rapid move to send X to the home position of 0.0 and Y to the home of 0.0 if you are working in inches that is 0.0" and in metric 0.0mm

    Here is one online overview that cover a lot of the basics.
    http://www.cnccookbook.com/CCCNCGCodeCourse.htm

    One great example of code you might need to tweak by hand, is when SheetCAM moves the torch between cuts. By default is will take the shortest path to the next cut, often going at a diagonal. If there are small parts that my have tipped up in the way the torch will crash into them. So you may want the torch to do the X move first then the Y move instead of both at once. So you will find the line with that move and break it into two lines. Like:

    original code:
    G0X14.750Y8.920

    new code:
    G0X14.750
    G0Y8.920
    Last edited by Rambozo; 01-02-2014 at 08:43 AM. Reason: add example
    Long arc, short arc, heliarc and in-the-dark!

  7. #7

    Default

    Yes I do have a switch on the floating head assembly. I have all of home and limit switches in series and it works fine. If I a not using the floating head I have a jumper plug that is to by-pass it in the table wiring. Mach treats the signal from the switches in a way you can do this. If you tell it to home it homes the Z first then the Y then the X so any switch trips will stop movement of the axis and goes to the next axis. Any switch tripped will stop movement on the table. When using a floating head switch mach is in that mode and when it touches the metal it says this is Z0.0 and backs up and continues the programmed steps to set the pierce height ect.

    Going back to X0 and Y0 the step before that should be to raise Z so the torch is out of the way as Rambozo said to be safe.

    Another thing is G0 is move fast and G1 is move under control of the last speed setting F and a number is telling mach how fast to move about. You will see and floating head operation with a low F number then when cutting command come up it will have a higher F number. Mach will operate at the last F speed until it is changed no matter what commands it is. See below.


    The arrows are pointing to speed commands and the box show a floating head routine touch the metal set Z to 0.0 move up to .25o” move down to .140 for pierce height M3 light the torch. Next line drop to .060” a f25 (cut height) next line start moving while cutting F200 all movements will be at 200 until told different. The N### are line numbers the mean nothing you can add command lines or remove line no problems.
    N15520 X2.0900 Y11.9293 I-1.1835 J-2.9238
    N15530 X2.0865 Y11.9097 I-0.0010 J-0.0100
    N15540 M05
    N15550 G00 Z1.0000
    G0Y0.0X0.0 added line to move back to start point
    N15560 M05 M30
    Attached Thumbnails Attached Thumbnails Click image for larger version. 

Name:	floating head parts (15).jpg 
Views:	1222 
Size:	139.0 KB 
ID:	11655  

    Everlast PM256
    Millermatic 180
    Hypertherm PowerMax 65 with machine torch
    Longevity Force Cut 80I
    DIY CNC table for plasma/routing
    13" metal lathe
    Small Mill
    ect, ect.

  8. Default

    So do I understand that a z micro switch is needed to allow touch to steel before each cut?
    I have a 1/4 inch of free movement on z axis .
    I may have to get a switch and find a place to mount it.
    maybe later I will send a few pictrues of my setup
    Wayne

  9. #9

    Default

    yes sir the Z limit and home switch is used to detect the end of travel for that axis. The floating head switch is only used to detect the metal when Mach tell the torch to go down and when it touches the metal that activates the switch and stops downward movement. Mach then resets the Z position to 0.0 and the torch moves back up until it reaches the Z value in the routine.
    It is hard to see but this video shows my table doing a touch routine.
    http://www.youtube.com/watch?v=gW7w9...mQfMwq0KTKpuRw

    Some table use a ohmic-sensing tip on the torch which works similar but only works on bare metal. And is a separate circuit just for that reason some manufactures still want a floating head switch as a backup for the ohmic-sensing tip so if it fail to make contact it don’t bust you torch????

    Everlast PM256
    Millermatic 180
    Hypertherm PowerMax 65 with machine torch
    Longevity Force Cut 80I
    DIY CNC table for plasma/routing
    13" metal lathe
    Small Mill
    ect, ect.

  10. Default

    I think that I will start by getting my proma thc to run.
    I will do a test run at near max amps and test the voltage display (hope to get close to 100volts) .
    to run the proma thc without the floating head (touch to metal) do I need a different post processor?
    I have a .4 second delay on the thc,
    I feel that the wiring and pin setup is okNow the holidays are over I can spend some time on my cnc machine.
    Thanks guys for the help, Many thanks to Acourtjester for spending time with this old newbie. It sure helps motivate me .
    Wayne

  11. #11

    Default

    Yes you may be able to run the mach3 plasma I think that was what I was running before floating head. You will still need to select THC so the signals from the THC control the torch movements. I would run the torch down to the surface and then zero out the Z DRO display and then move the torch up to maybe 1-1/2” off the surface to start you cutting. As long as you’re metal is not wrapped that should work to cut some parts.
    The floating head checks the surface each time you start a new cut and the THC keeps it at the cutting height as it moves around. It makes it so you don’t need to manual set Z0.0 each time.
    To set the THC volts do a straight line cut for a few inches and look at the volts on the THC to be an idea what you unit is working at you can do this without the THC turned one in Mach. If you have it one the THC may move the torch and then the volts will change and you will not get the correct volts for 0.060” cutting.
    You will get there and you learn many things along the way. Like many things the more you do the bigger the smile on your face becomes.

    Have fun
    Tom

    Everlast PM256
    Millermatic 180
    Hypertherm PowerMax 65 with machine torch
    Longevity Force Cut 80I
    DIY CNC table for plasma/routing
    13" metal lathe
    Small Mill
    ect, ect.

  12. Default

    Today I worked on the thc because my tractor didn't start to feed the cows .It is -50C WIND CHILL NOW.
    I will get them feed in the morning.
    I checked the raw voltage and it was around 52 at 47 amps on the pp50 ,65 psi air
    In config in mach3 I turned thc on.
    On the proma thc torch volts are 52,hys 4volts,d-t delay I changed to 1.5 second to allow the torch to fire and start,h-u volts are at 195volts.

    I had to play with the settings on thc on the mach3
    When I turned the thc on (green light) the torch wouldnot move once the torch fired.
    It seemed to work with it turned off.
    on the thc setting on mach3 I have
    -speed 10
    -max 2.0000
    -min -1.000 ( I had 0.000 but the torch wouldn't go down if I set the z at 0.00 to high)
    I may raise the raw volts up a little if the torch is cutting to low. (more testing) ;-)
    On that thought what is a good cut height for the pp50. I cant seem to find it out there.
    Also I would like a cutting chart for this machine, ( cut height, speed ipm,steel thickness, etc.)
    I hope now the tips will last longer.
    Over all had good progress today.
    Thanks all
    Wayne

  13. #13

    Default

    1/16" is a good height in general for cutting. 1/8" max.

  14. #14

    Default

    try two things there is a reset in the THC box click on it to clear out old setting.
    and upder ports & pins (mill options) no checks in the THC options boxs

    Everlast PM256
    Millermatic 180
    Hypertherm PowerMax 65 with machine torch
    Longevity Force Cut 80I
    DIY CNC table for plasma/routing
    13" metal lathe
    Small Mill
    ect, ect.

  15. Default

    I finished one sign . turned out ok .torch would cut out once in a while? I will try to attach picture .
    I will send a picture of my machine too if I can.
    Click image for larger version. 

Name:	cnc1.jpg 
Views:	454 
Size:	142.4 KB 
ID:	11696Click image for larger version. 

Name:	cnc2.jpg 
Views:	506 
Size:	147.3 KB 
ID:	11697Click image for larger version. 

Name:	cnc4.jpg 
Views:	571 
Size:	139.8 KB 
ID:	11698
    Maybe I may reduce the thc voltage a couple to lower the torch/
    wAYNE

  16. #16

    Default

    something that may help with cutting is to attach the work ground directly to the metal you are cutting.
    Here is a ground clamp I made for mine it is small and will not get in the way of cutting
    Attached Thumbnails Attached Thumbnails Click image for larger version. 

Name:	ground clamp (1).jpg 
Views:	269 
Size:	139.1 KB 
ID:	11699  

    Everlast PM256
    Millermatic 180
    Hypertherm PowerMax 65 with machine torch
    Longevity Force Cut 80I
    DIY CNC table for plasma/routing
    13" metal lathe
    Small Mill
    ect, ect.

  17. Default

    My plasma pp50 has a positive ground. And the rest of the machine has negative ground.
    my table is grounded to ground rod, and the pp50 ground clamp(which is positive is also clamped to table
    the table is all welded together and connected to all.
    when my consumables get bad the torch some times runs when it is moving from hole to hole and turns off when it
    is supposed to be cutting.
    off and on are switched.
    a new tip set seems to correct everything.
    (would this positive and negative table have issues here?)
    Wayne

  18. #18

    Default

    NO positive and negative thing is on everybody’s plasma table. After looking are the sign cut you have posted it looks like a cut path is interrupted from cutting. Lets say you are cutting a straight line and the torch stops cutting 1” out from the start and restarts at 2” and finishes the cut to the end. Only the torch goes out then relights but the table still does its motions. Is that what is happening with your table???? If so you need to look at the torch on signal maybe you have a bad relay. You say new consumables correct the problem do you feel you are getting good life from them? If not maybe you have water in the air.
    Post what you fine as this may help others down the road with their problems.

    Everlast PM256
    Millermatic 180
    Hypertherm PowerMax 65 with machine torch
    Longevity Force Cut 80I
    DIY CNC table for plasma/routing
    13" metal lathe
    Small Mill
    ect, ect.

Similar Threads

  1. Floating head Machine Torch holder w/ S45 Machine Torch - 2 for sale.
    By countryguy in forum Everlast Plasma Cutters (PAC)
    Replies: 2
    Last Post: 12-19-2016, 09:52 PM
  2. PP50 wont make second cut with out first turning machine off and on
    By xtreme cartz in forum Everlast Plasma Cutters (PAC)
    Replies: 33
    Last Post: 01-31-2013, 03:48 PM
  3. Having trouble with PP50
    By jtybt in forum Everlast Plasma Cutters (PAC)
    Replies: 11
    Last Post: 06-16-2011, 07:04 PM
  4. PP50 cup
    By jtybt in forum Everlast Plasma Cutters (PAC)
    Replies: 8
    Last Post: 04-21-2010, 04:54 AM
  5. New PP50 owner.
    By Nateh in forum Introduce Yourself
    Replies: 2
    Last Post: 01-11-2010, 10:04 PM

Posting Permissions

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