Word 'H' without required 'E' word

Results 1 to 15 of 15

Thread: Word 'H' without required 'E' word

  1. #1

    Default Word 'H' without required 'E' word

    Hello.

    I'm sorry to start another thread again, but I would need advice on one thing.

    I'm using Solidworks with Camworks and HAAS postprocesor for exporting gcode. However, each exported gcode displays a message when loaded into PlanetCNC. It says:

    GCode Error:Line:209 N1025 G00 G90 G53 G49 H0 Z0 M05
    D:\test.txt
    Word 'H' without required 'E' word

    What does it mean? What is "E" word? The problem is obviously in "H0". When I delete it, error message is gone. But I'm using tool changer and deleting all "H0" parameters make a mess on Z axis when changing tool.

    I was also looking for this sentence on internet but without succes.

    I would be grateful for any advice.

    Similar Threads:


  2. #2
    Member PlanetCNC's Avatar
    Join Date
    Mar 2017
    Location
    Slovenia
    Posts
    1295
    Downloads
    0
    Uploads
    0

    Default Re: Word 'H' without required 'E' word

    On HAAS G49 and H0 do same thing - cancel tool offset.
    So removing H0 should not change anything. But deleting a code without knowing what it does is wrong practice.

    It is no good idea to have everything in one line. It is often confusing and not properly understood.
    So lets break this:
    N1025 - This is just a line number and it does nothing - skip it
    G00 - Rapid Move. According to TNG g-code manual it also uses H and Z. Complete line is
    G00 H0 Z0 - this is clearly incorrect and that is why you get error.
    G90 - Distance Mode - Absolute
    G53 - Machine Coordinate System - this is nonmodal code and should be in same line as corresponding move
    G49 - Tool Offset Cancel
    M05 - Spindle Stop

    Now you need to reorder these lines to match desired order of execution
    G90 - modal state changes are first
    M05 - then spindle is stopped
    G49 - then all offsets are handled
    G53 G00 H0 Z0 - movement is last

    This is now much more human readable as before. And it is clearly visible why H0 cause an error.








  3. #3

    Default Re: Word 'H' without required 'E' word

    Hi.

    I'm sorry for late response. I'm quite busy at these day and I has just a litlle time to try it on the machine.

    So, thank you for detailed explanation. Unfortunately, the redesigned row still doesn't work. TNG still keeps rejecting him. But thanks to your explanation I notice one thing - there is two Tool Offset Cancel commands behind. G49 and H0. As I wrote before, deleting one of them makes a mess on Z axis during toll changes. But exchange G43 for G49 making TNG load the gcode correctly and also testing on the machine looks quite promissing. No more height mess on Z axis and tool change works good.
    I will need a litlle bit more time to test it. Just milling the air for first time, but this week I will try it on some plastic material and will let you known how it works.




  4. #4
    Member PlanetCNC's Avatar
    Join Date
    Mar 2017
    Location
    Slovenia
    Posts
    1295
    Downloads
    0
    Uploads
    0

    Default Re: Word 'H' without required 'E' word

    Using G43 instead of G49 is incorrect. You are enabling offset where it should be disabled. Is tooltable correctly set? How are you setting tool offset?



  5. #5
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Word 'H' without required 'E' word

    Quote Originally Posted by Jambolero View Post
    Hello.

    I'm sorry to start another thread again, but I would need advice on one thing.

    I'm using Solidworks with Camworks and HAAS postprocesor for exporting gcode. However, each exported gcode displays a message when loaded into PlanetCNC. It says:

    GCode Error:Line:209 N1025 G00 G90 G53 G49 H0 Z0 M05
    D:\test.txt
    Word 'H' without required 'E' word

    What does it mean? What is "E" word? The problem is obviously in "H0". When I delete it, error message is gone. But I'm using tool changer and deleting all "H0" parameters make a mess on Z axis when changing tool.

    I was also looking for this sentence on internet but without succes.

    I would be grateful for any advice.
    You need a tool number, if this is for a tool offset.

    If this is in the safety line, then it should not be there.

    When I look at that line, the whole line is messed up. what are you trying to achieve at that point in the program?

    Mactec54


  6. #6

    Default Re: Word 'H' without required 'E' word

    This my gcode, just a simple square 50x50x1mm in the center of stock 100x100x10mm. T01 is 6mm cutter.
    Tool crib is set in Camworks (SolidWorks). Postprocessor is HAAS_VF3 which is included in Camworks by default.

    %
    O00001
    N5 G21 G17 G40 G80 G90
    N10 T01 M06
    N15 G54 G90 G94
    N20 S25000 M03
    N25 G90 G42 D01 G00 X72. Y28.
    N30 G43 H01 Z1. M07
    N35 G01 Z-1. F30.
    N40 X28. F1200.
    N45 Y72.
    N50 X72.
    N55 Y28.
    N60 Z1. F500. M09
    N65 G40 G00 X72. Y28.
    N70 G00 G90 G53 G49 H0 Z0 M05
    N75 G54 X0 Y0
    N80 M30
    %

    In Camworks I have tool crib with with 17 fully defined tools. In TNG Tool table I create 17 tools, where only written values are XYZ position for tool change and tool offset, which is written automatically after tool is measured on probe during tool change sequence.

    So the TNG knows the tool number and corresponding offset and everything else is care of gcode.

    And as I wrote before, the problem is in the line with H0. TNG simply refuses to load it. But changing G49 to G43 works. I don't known why, but it works. And of course I didn't change anything in M06 script.



  7. #7
    Member PlanetCNC's Avatar
    Join Date
    Mar 2017
    Location
    Slovenia
    Posts
    1295
    Downloads
    0
    Uploads
    0

    Default Re: Word 'H' without required 'E' word

    Like I said:
    G49 disables tool offset. Which is logical thig to do before tool change and at end of program.
    G49 H0 is wrong syntax. TNG uses just G49. H0 is then used with G00 which makes no sense in this context.
    G43 enables tool offset.
    G43 H0 also enables tool offset.

    Recheck your offsets. You can export your profile and send it (zip file) to our support.

    PS
    I'll modify g-code interpreter so that G49 H0 will be accepted. But this will not solve your problem.



  8. #8

    Default Re: Word 'H' without required 'E' word

    Mail with configuration file has been sent.



  9. #9
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Word 'H' without required 'E' word

    Quote Originally Posted by PlanetCNC View Post
    Using G43 instead of G49 is incorrect. You are enabling offset where it should be disabled. Is tooltable correctly set? How are you setting tool offset?
    G49 and H0 should not be used, there is never a need to cancel tool offsets. unless you are using a 5axis machine

    M30 cancels any H value Tool Offset at the end of a program.

    Mactec54


  10. #10
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Word 'H' without required 'E' word

    Quote Originally Posted by Jambolero View Post
    This my gcode, just a simple square 50x50x1mm in the center of stock 100x100x10mm. T01 is 6mm cutter.
    Tool crib is set in Camworks (SolidWorks). Postprocessor is HAAS_VF3 which is included in Camworks by default.

    %
    O00001
    N5 G21 G17 G40 G80 G90
    N10 T01 M06
    N15 G54 G90 G94
    N20 S25000 M03
    N25 G90 G42 D01 G00 X72. Y28.
    N30 G43 H01 Z1. M07
    N35 G01 Z-1. F30.
    N40 X28. F1200.
    N45 Y72.
    N50 X72.
    N55 Y28.
    N60 Z1. F500. M09
    N65 G40 G00 X72. Y28.
    N70 G00 G90 G53 G49 H0 Z0 M05
    N75 G54 X0 Y0
    N80 M30
    %

    In Camworks I have tool crib with with 17 fully defined tools. In TNG Tool table I create 17 tools, where only written values are XYZ position for tool change and tool offset, which is written automatically after tool is measured on probe during tool change sequence.

    So the TNG knows the tool number and corresponding offset and everything else is care of gcode.

    And as I wrote before, the problem is in the line with H0. TNG simply refuses to load it. But changing G49 to G43 works. I don't known why, but it works. And of course I didn't change anything in M06 script.
    Just change it like this at the bottom the rest is ok


    %
    O00001
    N5 G21 G17 G40 G80 G90
    N10 T01 M06
    N15 G54 G90 G94
    N20 S25000 M03
    N25 G90 G42 D01 G00 X72. Y28.
    N30 G43 H01 Z1. M07
    N35 G01 Z-1. F30.
    N40 X28. F1200.
    N45 Y72.
    N50 X72.
    N55 Y28.
    N60 Z1. F500. M09
    N65 G40 G00 X72. Y28.
    N70 G0Z0
    M05
    N75 G53 X0 Y0 (Not G54)
    N80 M30
    %

    Mactec54


  11. #11
    Member PlanetCNC's Avatar
    Join Date
    Mar 2017
    Location
    Slovenia
    Posts
    1295
    Downloads
    0
    Uploads
    0

    Default Re: Word 'H' without required 'E' word

    N70 G0Z0 should be N70 G53G0Z0. Assuming that safe Z is at Z0 which is common practice. Otherwise it makes no sense.



  12. #12
    Member PlanetCNC's Avatar
    Join Date
    Mar 2017
    Location
    Slovenia
    Posts
    1295
    Downloads
    0
    Uploads
    0

    Default Re: Word 'H' without required 'E' word

    I checked your profile. Tool Change settings are wrong. If you are using G43 and G49 in g-code the you should not set offset from within tool change.



  13. #13

    Default Re: Word 'H' without required 'E' word

    Quote Originally Posted by PlanetCNC View Post
    I checked your profile. Tool Change settings are wrong. If you are using G43 and G49 in g-code the you should not set offset from within tool change.
    Its true that we have a really hard time to find correct settings for tool changing. This was only one which works. Can you be please more specific what is wrong in the settings?

    Anyway I used corrected gcode from mactec54 ( thank you very much ) and it really works. With exception of G53 Z0 instead G00 Z0 at the end of the blocks. Now the code with three tool changes and same object looks like this:

    %
    O00001


    N5 G21 G17 G40 G80 G90
    N10 T01 M06 (6/6 1-tooth Al VHF)
    N15 G54 G90 G94
    N20 S25000 M03
    N25 G90 G42 D01 G00 X72. Y28.
    N30 G43 H01 Z1. M07
    N35 G01 Z-1. F30.
    N40 X28. F1200.
    N45 Y72.
    N50 X72.
    N55 Y28.
    N60 Z1. F500. M09
    N65 G40 G00 X72. Y28.
    N70 G53 Z0
    M05


    N75 T02 M06 (3/6 1-tooth Al VHF)
    N80 G54 G90 G94
    N85 S28000 M03
    N90 G90 G42 D02 X73.5 Y26.5
    N95 G43 H02 Z1. M07
    N100 G01 Z-1. F72.
    N105 X26.5 F1019.2
    N110 Y73.5
    N115 X73.5
    N120 Y26.5
    N125 Z1. F500. M09
    N130 G40 G00 X73.5 Y26.5
    N135 G53 Z0
    M05


    N140 T04 M06 (2/6 1-tooth Al VHF)
    N145 G54 G90 G94
    N150 S34000 M03
    N155 G90 G42 D04 X74. Y26.
    N160 G43 H04 Z1. M07
    N165 G01 Z-1. F72.
    N170 X26. F1200.
    N175 Y74.
    N180 X74.
    N185 Y26.
    N190 Z1. F500. M09
    N195 G40 G00 X74. Y26.
    N200 G53 Z0
    M05
    N205 G54 X0 Y0
    N210 M30
    %


    So far so good. All tools are milling in the same height so the tool offset should work ( somehow ).



  14. #14
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: Word 'H' without required 'E' word

    Quote Originally Posted by Jambolero View Post
    Its true that we have a really hard time to find correct settings for tool changing. This was only one which works. Can you be please more specific what is wrong in the settings?

    Anyway I used corrected gcode from mactec54 ( thank you very much ) and it really works. With exception of G53 Z0 instead G00 Z0 at the end of the blocks. Now the code with three tool changes and same object looks like this:

    %
    O00001


    N5 G21 G17 G40 G80 G90
    N10 T01 M06 (6/6 1-tooth Al VHF)
    N15 G54 G90 G94
    N20 S25000 M03
    N25 G90 G42 D01 G00 X72. Y28.
    N30 G43 H01 Z1. M07
    N35 G01 Z-1. F30.
    N40 X28. F1200.
    N45 Y72.
    N50 X72.
    N55 Y28.
    N60 Z1. F500. M09
    N65 G40 G00 X72. Y28.
    N70 G53 Z0
    M05


    N75 T02 M06 (3/6 1-tooth Al VHF)
    N80 G54 G90 G94
    N85 S28000 M03
    N90 G90 G42 D02 X73.5 Y26.5
    N95 G43 H02 Z1. M07
    N100 G01 Z-1. F72.
    N105 X26.5 F1019.2
    N110 Y73.5
    N115 X73.5
    N120 Y26.5
    N125 Z1. F500. M09
    N130 G40 G00 X73.5 Y26.5
    N135 G53 Z0
    M05


    N140 T04 M06 (2/6 1-tooth Al VHF)
    N145 G54 G90 G94
    N150 S34000 M03
    N155 G90 G42 D04 X74. Y26.
    N160 G43 H04 Z1. M07
    N165 G01 Z-1. F72.
    N170 X26. F1200.
    N175 Y74.
    N180 X74.
    N185 Y26.
    N190 Z1. F500. M09
    N195 G40 G00 X74. Y26.
    N200 G53 Z0
    M05
    N205 G54 X0 Y0
    N210 M30
    %


    So far so good. All tools are milling in the same height so the tool offset should work ( somehow ).
    Your tool offsets are controlled by G43H04, G43H02 and G43H01, this will look at T4 / T2 and T1 in the tool table an apply whatever the Offset you have set for that tool.

    N205 G54X0Y0. this should be N205 G53X0Y0

    G00 or G0 either should work.

    You have to be careful how you us a G53 as it needs a G00 on the same line or one before it or it will not work

    Because you used a G00 online N195 then it will work, if that G00 was not there it most likely will not work.

    Mactec54


  15. #15

    Default Re: Word 'H' without required 'E' word

    Good point mactec54. Thanks.

    I'll take a look at that. I'll make a few changes to the postprocessor.

    Anyway TNG works very well with modified gcode according ti this thread. Thank you guys.



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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Word 'H' without required 'E' word

Word 'H' without required 'E' word