Proxxon CNC Mill and nccad9 software

Discussion in 'Software and Programming' started by Lofty76, Feb 10, 2018.

Help Support HMEM by donating:

  1. Feb 10, 2018 #1

    Lofty76

    Lofty76

    Lofty76

    Member HMEM Supporter

    Joined:
    Jun 6, 2013
    Messages:
    9
    Likes Received:
    0
    Gender:
    Male
    Occupation:
    Technician Engineer (Rotary Wing)
    Location:
    UK, South Coast
    Hello everybody, Recently, in an attempt to get up to date I purchased the above in order to learn some basic cnc programming.Unfortunately the nccad software is mostly in german and support from Max computers (the vendors) is not overly forthcoming. I want to try and learn to manufacture loco nameplates - the ones with raised letters, for a start project.
    Can anyone recommend software that will work with the machine and that I can understand?

    Many thanks for your help in advance

    Regards

    Lofty
     
  2. Feb 11, 2018 #2

    kvom

    kvom

    kvom

    Administrator Staff Member Administrator Global Moderator

    Joined:
    Jun 4, 2008
    Messages:
    3,135
    Likes Received:
    588
    I took a look at the nccad/max website. As far as I can tell nccad is a cam program that works only with imported STL 3D files. 3D machining is probably not what you want for something like nameplates.

    Does your machine have a separate control program like Mach3?
     
  3. Feb 11, 2018 #3

    Lofty76

    Lofty76

    Lofty76

    Member HMEM Supporter

    Joined:
    Jun 6, 2013
    Messages:
    9
    Likes Received:
    0
    Gender:
    Male
    Occupation:
    Technician Engineer (Rotary Wing)
    Location:
    UK, South Coast
    Many thanks for your reply.

    The program seems fine for standard engraving, I have worked out to input the machine limits / parameters, setting tool zero height etc, and then running a simple text program ( using a pencil in the machine collet on card clamped to the table), probably not the best way forward but I am beginning to understand the way things work.

    I did find a program called VCarve which shows exactly what I want to do. but I can't control the machine from it, the only way that I could see was to export the vcarve code into the nccad program as the trial version of vcarve doesn't allow export directly to the machine.

    Does Mach 3 have a usable trial?
     
  4. Feb 11, 2018 #4

    kvom

    kvom

    kvom

    Administrator Staff Member Administrator Global Moderator

    Joined:
    Jun 4, 2008
    Messages:
    3,135
    Likes Received:
    588
    As long as g-code can be imported to the control that's the way to go.
     
  5. Feb 18, 2018 #5

    Lofty76

    Lofty76

    Lofty76

    Member HMEM Supporter

    Joined:
    Jun 6, 2013
    Messages:
    9
    Likes Received:
    0
    Gender:
    Male
    Occupation:
    Technician Engineer (Rotary Wing)
    Location:
    UK, South Coast
    Thanks Kvom, Mach 3 works a treat, much obliged.
     
  6. Sep 23, 2018 #6

    Chris Alderson

    Chris Alderson

    Chris Alderson

    Member

    Joined:
    Sep 23, 2018
    Messages:
    15
    Likes Received:
    0
    Gender:
    Male
    Location:
    Whitley bay england
    Lofty76

    I currently have the same problem you where experiencing, I have just purchased the proxxon ff 500 cnc which comes with nccad9

    However the software that is provided with the system is only the basic version with lots of restrictions, I have looked in to upgrading it to the full version which is going to cost another £290 that's without shipping as you can't download it they have to send you a CD probably because they charge you another 280 euros for international shipping.

    Any advice on software alternatives or just a direction to head in here would be a life saver because nccad9 basic is just about unusable and has no 3d functions or useful help.

    Any assistance will be greatly appreciated

    Chris
     
  7. Sep 23, 2018 #7

    Bazzer

    Bazzer

    Bazzer

    Member

    Joined:
    May 14, 2017
    Messages:
    17
    Likes Received:
    0
    Chris

    I have a Wabeco CC F1210 mill that runs with NCCAD 7.5, I get a lot of work out of the machine and NCCAD.

    I do not however try to do any 2D or 3D CAD within NCCAD, just regard NCCAD as a machine control like Mach3 or Eding and import G code generated by another CAD/CAM program.

    You will not be able to get anything like Mach3 to drive the Max computer controls, they have that side of things locked down very tightly.

    The accepted G codes for NCCAD are fairly limited, however you will be able to make the machine do just about anything that you want, you will have to get a post processor sorted out if you do use another CAD/CAM to generate designs and G code.

    I did have a little communication with Max Computer about 3D capabilities and in his very broken english he said anything complicated to generate outside of NCCAD and import the G code.

    Anyhelp or sample code required then just drop me a line, I am 99% certain that the code is identical for the wabeco and proxxon versions.

    Regards

    Barrie
     
  8. Sep 23, 2018 #8

    Chris Alderson

    Chris Alderson

    Chris Alderson

    Member

    Joined:
    Sep 23, 2018
    Messages:
    15
    Likes Received:
    0
    Gender:
    Male
    Location:
    Whitley bay england
    Hi Barrie

    Thank you for replying

    The version of nccad9 I have received with the proxxon FF500/bl cnc is nccad9 basic which has very limited usability.

    You cant import stl files, you can only open 1 file at a time, and you cant generate anything over 5000 sentences as they put it.

    Currently I have tried simple engraving and never get past the first letter, I get an error message, and there is nothing to check this error message against, nothing about it in the help directory which is honestly useless as it refers to the full version of nccad9.

    I have looked in to upgrading nccad9 to the full version which I really shouldn't have to do as I've paid over £5000 for this machine and software and the cost including shipping would be well over 500 euros because you cant just download it from them they have to ship to to you, which I'm definitely not going to pay on top of what I already have.

    I posted on here as it seems Lofty76 got some joy with Mach3 ?

    Regards

    Chris
     
  9. Sep 23, 2018 #9

    Bazzer

    Bazzer

    Bazzer

    Member

    Joined:
    May 14, 2017
    Messages:
    17
    Likes Received:
    0
    Hello Chris

    5000 lines maybe a limitation, I dont do engraving so I dont know how many letters 5000 lines buy you.

    I bought the hand pendant direct from Max computer, they dont charge the 280 euros shipping, I think that is to cover themselves for tricky exports, get a shipping quote from them, it will be 20 euro's or similar.

    I would definately be interested to know if some one has the key to get the Max computer control working with Mach 3 but I am not holdig my breath on that one.

    The best thing to do is make the mill follow a really simple programme to start with, that proves everythings out.

    G91
    G00 x100
    y30
    x-100
    y-30

    Create the above programme in notepad or similar and save the file with the extension *.KNC, so change the file you create in Notepad from having *.txt to KNC. Set your machine zero point so as that there is plenty of movement avaliable in the positive X axis (table quite well over to the right) and with the table fairly close to you to allow movement in the Y axis, leave the Z axis up high. Zero the machine by pressing ctrl X, then ctrl Y and finally ctrl Z.

    Now open the above created file and press the go button and see what happens. If you get this going I can walk you through getting a bit more adventurous !!

    I hate to say this but you have to get this working, I will bet you that it is not possible to get the controls working with Mach 3 so you have to keep going. I use the NCCAD controlled Wabeco more or less every day, there is a learning curve but it is all possible. I do mostly 3D machining of stainless steel. Where did you buy the mill from?

    Regards

    Barrie
     
  10. Sep 23, 2018 #10

    Chris Alderson

    Chris Alderson

    Chris Alderson

    Member

    Joined:
    Sep 23, 2018
    Messages:
    15
    Likes Received:
    0
    Gender:
    Male
    Location:
    Whitley bay england
    Hi Barrie

    I have done as you advised, the 5000 lines is for any job engraving was just a quick test of the machine to see if it functioned as expected but didn't work, as soon as the first letter is machined the program throws up a z axis invalid move error and ends, I tried this with basic shapes and get exactly the same result, z axis movement error.

    There is nothing to refer to for causes of this error at least not that is in English.

    The code you game me made the x and y axis move, looked like the table was stencilling out a rectangle, no movement on the Z axis at all.

    Regards

    Chris
     
  11. Sep 23, 2018 #11

    ThomasSK

    ThomasSK

    ThomasSK

    Well-Known Member

    Joined:
    Aug 9, 2014
    Messages:
    45
    Likes Received:
    5
    Location:
    South East Norway
    What is your safe Z set to? lets say you have a mill with 200mm of Z travel, and you send it a g-code like "Z-1000" then your controller may throw a error like that.

    I'd recommend reading one of the basic courses of programming G-code. With the cheat list of M and G codes, its fairly easy to do the basic shapes, and its quote helpful when you are fault finding a program.

    As a test, lets try this program:
    Code:
    G21
    G90
    M3 S1000
    G00 X0 Y0 Z0
    G01 Z-1
    G01 X10
    G01 Y10
    G01 X0
    G01 Y0
    G00 Z-10
    M5
    M30
    This should start in one corner, start the spindle at 1000 rpm, go down 1mm, then go 10mm in X, then 10mm in Y, then back to make it a square.
    I'm not sure that the proxxon has control of the spindle from the controller, in that case, remove the S1000 from line 3.

    Wikipedia has a good list of what the codes means

    BR.
    Thomas.
     
  12. Sep 23, 2018 #12

    Bazzer

    Bazzer

    Bazzer

    Member

    Joined:
    May 14, 2017
    Messages:
    17
    Likes Received:
    0
    Thomas

    This machine has a funny implimemtation of DIN ISO G codes, it will not start or stop the spindle with M3 and M5, G21 will not be recognised, M30 will throw it as well as they use M30 as a pause and then you specify the time delay of the pause.

    Spindle start is M10 o6.1 and stop is M10 o6.0

    The characters in front of the 6's above are letter 'O' for output.

    Very strange controls but used by two well respected German manufacturers, go figure.

    Best Regards

    Barrie
     
  13. Sep 23, 2018 #13

    kf2qd

    kf2qd

    kf2qd

    Well-Known Member

    Joined:
    Apr 1, 2008
    Messages:
    477
    Likes Received:
    36
    Can you tell uswhat G and M codes the machine accepts? And what CAD system you might have experience with?
     
  14. Sep 23, 2018 #14

    Bazzer

    Bazzer

    Bazzer

    Member

    Joined:
    May 14, 2017
    Messages:
    17
    Likes Received:
    0
    Hello Chris

    As Thomas eluded to the Z axis error you are getting is likely to do with the Z zero and travels conflicting.

    So set the Z zero with the Z axis about half way up the Z travel movement.

    Now run this code

    G91
    G00 X0 Y0 Z0
    Z -10
    x100
    y30
    x-100
    y-30
    z 10

    You will see the same rectangle as before but the Z axis will drop 10mm at the start and raise 10mm at the end.

    Also as a seperate programme try this

    M10 O6.1
    M30 p180
    M10 O6.0

    This programme starts and stops the spindle with the Wabeco mill, it might be different for Proxxon, let us know what the results are of the spindle test, M10 is relay controls in NCCAD speak. 'O' (letter O) is output 6.1 is relay 'on' and 6.0 is relay 'off'. M30 is pause and the P180 is pause for ten seconds, they split a second down into 18th's so 10x18 equals 180.

    With the Wabeco the spindle speed is set manually, I think the Proxxon is the same looking at the photo's.

    If the above is all ok then I think we should cut some material, do you have some 3mm plywood? what cutters do you have? Looking at the spec of the machine on the Proxxon website it looks like the spindle RPM is max 2500 rpm, is that your understanding? I see they offer a bracket to get a high RPM spindle mounted, that sounds like a good idea to me.

    One step at a time as they say!!

    Best Regards

    Barrie
     
  15. Sep 24, 2018 #15

    Chris Alderson

    Chris Alderson

    Chris Alderson

    Member

    Joined:
    Sep 23, 2018
    Messages:
    15
    Likes Received:
    0
    Gender:
    Male
    Location:
    Whitley bay england
    Hi Barrie

    I loaded the program in to nccad it seems the pieces of code for the Z axis movement had spaces in as the system gave an error for each line, I've taken the spaces out and all seems to be ok.

    The code ran fine Z dropped, X and Y made a rectangle but when Z was returning to the 0 point it ran very slowly, no doubt this is a setting somewhere ?

    kf2qd I currently have no experience with G-code other than the above Barrie has kindly shown me, I'm only just getting in to CNC so baby steps at the moment, I have used google SketchUp quite a bit, years a go I used 3ds max but that was a good while back.

    I have been looking in to different CAD programs to use for design then being able to import in to nccad9 but because of the restrictions on nccad9 basic I'm not really able to do this, plus forgive me if I'm wrong but nccad doesn't really seem compatible with other programs ? perhaps this is just the fact I'm using the basic version ?

    Thank you for replying to me so promptly everyone, I didn't think I would receive a response so soon never mind all the help I'm receiving plus the G-code lessons im getting from Barrie.

    Regards

    Chris
     
  16. Sep 24, 2018 #16

    Bazzer

    Bazzer

    Bazzer

    Member

    Joined:
    May 14, 2017
    Messages:
    17
    Likes Received:
    0
    Hello Chris

    Not sure why it went slowly in the Z rectract, once G00 is invoked (rapid movement) the machine should stay in that speed until G01 is invoked (G01 is move at cutting speed) we did not call up G01, so that is strange. Did you get to try the spindle start and stop programme yet? and did you get a chance to look for materials and cutters?

    Let me know if you wish to continue this remote tutorial and we should be able to get 2.5D cutting going quite easily, then maybe flip back to trying the engraving within NCCAD.

    NCCAD is not the most friendly programme to start with but you can get things done with it, Wabeco and Proxxon sell a good number of machines with this software.

    Out of interest where did you buy the Proxxon machine?

    Best Regards

    Barrie
     
  17. Sep 24, 2018 #17

    Chris Alderson

    Chris Alderson

    Chris Alderson

    Member

    Joined:
    Sep 23, 2018
    Messages:
    15
    Likes Received:
    0
    Gender:
    Male
    Location:
    Whitley bay england
    Hi Barry

    I believe it may be a setting somewhere.

    Yes the spindle program worked fine no X,Y or Z movement just spindle on and off, so from that I'm getting M10 O6.1 tells the MCS control unit to close relay 6 (Close contact) and M10 O6.0 open relay 6 (Open contact).

    I have Aluminium sheet, loads of scrap pieces of Pine, Steel square bar, Brass round bar.

    Endmill cutters HSS 6, 7, 8, 10mm 4 flute / Tungsten carbide 6mm 4 flute and proxxon milling cutter set 1, 2, 3mm 2 flute
    I also have a few other cutters Axminister's own make they are more like rasp cutters though.

    I bought the machine from Axminster tools and machinery.

    By all means Barrie please continue the tutorials as it is really helping with my understanding of the CNC machine and how G-code works in relation to it.

    Regards

    Chris
     
  18. Sep 24, 2018 #18

    Bazzer

    Bazzer

    Bazzer

    Member

    Joined:
    May 14, 2017
    Messages:
    17
    Likes Received:
    0
    Hello Chris

    Your understanding of M10 and the relay sense is perfect. I take it that the speed of the spindle is set manually?

    If you want to cut a part, I would propose a rectangle with a circle or ellipse cut out of the middle. Given that the machine is new and feed rates are a bit of an unknown I would strongly suggest cutting some plywood or similar material to start with. you have cutters listed that would be just fine for this test. We do need to know the thickness of the work piece material if we are going to cut it free. Alternatively we could mount a lump of pine into the vise if you have one and work away above the vice jaws.

    If we do a flat sheet job we will need a sacrificial board underneath the work piece, 10mm ply or MDF is good for this, but you need some kind of clamp system to hold the boards down onto the machine table.

    I looked at some videos of the machine that you have on Youtube doing engraving, the machine seemed quite capable.

    Let me know on the questions above and I will get something programmed up for you.

    Best Regards

    Barrie
     
  19. Sep 24, 2018 #19

    Chris Alderson

    Chris Alderson

    Chris Alderson

    Member

    Joined:
    Sep 23, 2018
    Messages:
    15
    Likes Received:
    0
    Gender:
    Male
    Location:
    Whitley bay england
    Hi Barrie

    Yes the speed of the spindle is set manually on the front of the machine head, it peaks at 4000 rpm.

    That would be great Barrie if it is not too much trouble, I can get the material ready, also I have a set of step clamps to hold in place.

    Yes I have probably watched the same videos however I now know the 5000 sentence limitation of nccad9 which I managed to fill with one 5 letter word at a 2mm depth which I find ridiculous, I did speak to proxxon via email earlier on today and they tried to advise me they have only provided basic to try and keep the cost of the machine down. They also went on to say that it should satisfy most tasks other than the use of STL files. Guessing the gent who emailed me has not yet tried to engrave on basic..

    While I was making my discovery earlier I received that "invalid movement z axis" message again and from what I can gather it is happing somewhere in these lines of code:

    G01 X48.965 Y30.284
    G01 X48.130 Y30.360
    G00 Z5.000
    G00 Z0.500
    G01 Z-2.000 F5.000
    G01 X48.320 Y30.990 F50.000
    G01 X59.790
    G01 X59.600 Y30.360
    G01 X58.996 Y30.331

    Any ideas what could be causing this error Barrie ?

    Regards

    Chris
     
  20. Sep 24, 2018 #20

    Bazzer

    Bazzer

    Bazzer

    Member

    Joined:
    May 14, 2017
    Messages:
    17
    Likes Received:
    0
    Hello Chris

    Lets look at what the code is telling the machine to do.

    G01 X48.965 Y30.284 This line is a cutting action, assume the tool is cutting and it is going to X 48.965 and Y 30.284
    G01 X48.130 Y30.360 Cutting action again with a very small movement relative to the last line
    G00 Z5.000 This is a rapid movement pulling up in the Z axis 5mm away from the zero point
    G00 Z0.500 This is a rapid movement but looks to be 0.5mm above the work piece.
    G01 Z-2.000 F5.000 This a cutting/plunge action into the work piece at a feed of 5.0 (actually 30mm/min)
    G01 X48.320 Y30.990 F50.000 Cutting in the X,Y plane with cutter at the depth from the previous line feed of 300mm/min
    G01 X59.790 Cutting movement just in the X axis
    G01 X59.600 Y30.360 Cutting movement
    G01 X58.996 Y30.331 Cutting movement

    Another qwerk of the Max computer control is that the feed rate (F after a cutting operation such as G01) unit is 0.1mm per second rather than the more convemntional units of 1mm second. so F5 in your code is 0.5mm per second which works at the more conventionally quoted figure of 30mm/min. Basically multiply Max computer feed by 6 to get a mm/min figure.

    I see nothing outlandish in your code but if you had the Z zero set very close to either the top or bottom of Z axis travel, then one of the Z axis movement requests could push the machine out of limits and result in the error message. Try running the code again but set the Z axis zero right in the middle of the travel. Have you got the Z zero set very low on the Z axis, maybe a very short cutter has forced you to do this?

    I assume the code was some sort of engraving or text?

    Did you speak to Axminster about any of this? I would be interested to know if they have someone down there who understands the qwerks of Max computer controls?

    I will figure out the programme tomorrow but feel free to ask any questions that come to mind before then.

    Best Regards

    Barrie
     

Share This Page