UCCNC G53 or G54

Results 1 to 16 of 16

Thread: UCCNC G53 or G54

  1. #1
    Gold Member daniellyall's Avatar
    Join Date
    Sep 2009
    Location
    New Zealand
    Posts
    1856
    Downloads
    3
    Uploads
    0

    Default UCCNC G53 or G54

    Are there any issues useing G53 or G54 in UCCNC

    (1001)
    (TEST 4 AXIS)
    (T3 D=10. CR=0. - ZMIN=-10.1 - FLAT END MILL)
    G90 G94 G91.1 G40 G49 G17
    G21
    G53 Z0.
    G90

    or

    (1001)
    (TEST 4 AXIS)
    (T3 D=10. CR=0. - ZMIN=-10.1 - FLAT END MILL)
    G90 G94 G91.1 G40 G49 G17
    G21
    G54 Z0
    G90

    And haveing G54 Z0 at the end instead of G53 Z0 or G28/G30 Z0 at the end.

    Similar Threads:
    <img src="https://ivxo1q-dm2305.files.1drv.com/y4mENMmTr_Cabc7pR0FUdB6gtbADq2JbuG4_rGy0eBQvLJx19pTi6TqMUIJN0xgOyDIc0gWoxYhS38HpbSTFGdfaK-o42IOU6jczrhDpfpCOTNGL1X6hvZCbgj0y35gqmq1YGTrWwShYGV-C7lXA2esy0Pi_WfnBSyroDLSGXwce4uSr1U7op7srdi78rispHCa_K4aFlTlJPVkkNWMfgh_Tg?width=60&height=60&cropmode=none" width="60" height="60" />

    Being Disabled is OK CNC is For fuN


  2. #2
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: UCCNC G53 or G54

    I'm assuming you are creating or editing a Fusion 360 post?

    G53 Z0
    G54 Z0
    Neither of these lines actually do anything.

    Do you mean G0 G53 Z0?
    Personally, I remove that from my post. I don't want the machine to rapid all the way up at the start of my code.
    I also wouldn't want a G0 G54 Z0, as that could cause a crash.

    Also, G94, G91.1, G21, and G20 are not used in UCCNC. (Hopefully G94 will in the future, if the often requested G93 is added.)

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

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

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


  3. #3
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Quote Originally Posted by daniellyall View Post
    Are there any issues useing G53 or G54 in UCCNC

    (1001)
    (TEST 4 AXIS)
    (T3 D=10. CR=0. - ZMIN=-10.1 - FLAT END MILL)
    G90 G94 G91.1 G40 G49 G17
    G21
    G53 Z0.
    G90

    or

    (1001)
    (TEST 4 AXIS)
    (T3 D=10. CR=0. - ZMIN=-10.1 - FLAT END MILL)
    G90 G94 G91.1 G40 G49 G17
    G21
    G54 Z0
    G90

    And haveing G54 Z0 at the end instead of G53 Z0 or G28/G30 Z0 at the end.
    G53 and G54 are ( 2 ) very different Codes

    G54 through G59 Plus can only be used for your work offset

    A G53 can be used but not normally for a first move in your program and is normally use with a G0G53, if a G0 is active Like I show at the end of the program, then it can be used by it's self G53, not all controls support the use a G53

    G0Z100.
    G53X---Y---


    %
    (1001)
    (TEST 4 AXIS)
    (T3 D=10. CR=0. - ZMIN=-10.1 - FLAT END MILL)

    G90 G94 G91.1 G40 G49 G17 ( G94 and G49 is not needed in this line add a G80 )
    G21

    (T1M6 Tool number 1 This Line can be replaced with a safety Z axes move if you don't have a Tool Changer as below )

    G0Z100. ( It will move the Z axes, 100mm above the work, if everything has been setup correct, this only works if you have homed your machine correctly ) ( you can use any number you want )

    M8 ( only needed if you have coolant or an air blow Etc )

    G54 ( Work offset X0 Y0 start position of your work )

    G90G0X-----Y------- ( where you are going to start cutting )

    G43Z.1H1 ( G43 is your Tool offset Z axes will move to .1 above the part, this can be any number you want, H1 is your tool in the offset page )

    G1Z-0.06 ( this is the start of your program you are going to cut )

    G90 ( you have G90 in the Header so this is not needed again unless you use a G91 after a G90, if you use a G91 you must have a G90 for the next move after it's use, one cancels the other )


    End of program

    G0Z100. ( Z axes moves up 100mm to clear your work )

    M9 ( if you have coolant to shut off )

    M5 ( Turns spindle off )

    G53X------Y-------- ( Moves to where ever you want your part to be )
    %

    Mactec54


  4. #4
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Quote Originally Posted by ger21 View Post
    I'm assuming you are creating or editing a Fusion 360 post?


    Neither of these lines actually do anything.

    Do you mean G0 G53 Z0?
    Personally, I remove that from my post. I don't want the machine to rapid all the way up at the start of my code.
    I also wouldn't want a G0 G54 Z0, as that could cause a crash.

    Also, G94, G91.1, G21, and G20 are not used in UCCNC. (Hopefully G94 will in the future, if the often requested G93 is added.)
    What is the use of a G93, I don't know of any time you would have a need for it, G94 and G95 are the only 2 feed codes that used for everyday use


    Do people even know what inverse time mode means

    G93, Inverse Time Mode ON, translates the linear (inches/mm) feedrate into a value that takes rotary motion into account. G93 specifies that all F (feed rate) values are interpreted as strokes per minute. In other words, the time (in seconds) to complete the programmed motion using G93 is 60 (seconds) divided by the F value.

    Mactec54


  5. #5
    Gold Member daniellyall's Avatar
    Join Date
    Sep 2009
    Location
    New Zealand
    Posts
    1856
    Downloads
    3
    Uploads
    0

    Default Re: UCCNC G53 or G54

    It's more I just needed to know if G54 was a bad idea at the start and end of the G code for UCCNC yes ger G0 G54 Z0

    The newest UCCNC post for fusion has G53 one of the UCCNC users wonted his changed from G53 to G54 at the start and end.

    I will let him know that have G54 could cause a crash and where it goes its up to him to test it.

    mactec54 the chunk of G Code I posted is not the header from the UCCNC post it just has G90 in it, that was what I had open at the time I posted here.

    I know what G93, G94 and G95 are for

    <img src="https://ivxo1q-dm2305.files.1drv.com/y4mENMmTr_Cabc7pR0FUdB6gtbADq2JbuG4_rGy0eBQvLJx19pTi6TqMUIJN0xgOyDIc0gWoxYhS38HpbSTFGdfaK-o42IOU6jczrhDpfpCOTNGL1X6hvZCbgj0y35gqmq1YGTrWwShYGV-C7lXA2esy0Pi_WfnBSyroDLSGXwce4uSr1U7op7srdi78rispHCa_K4aFlTlJPVkkNWMfgh_Tg?width=60&height=60&cropmode=none" width="60" height="60" />

    Being Disabled is OK CNC is For fuN


  6. #6
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: UCCNC G53 or G54

    What is the use of a G93, I don't know of any time you would have a need for it,
    Rotary axis work using G93 makes it easy to get the proper feedrates on the rotary axis moves on controls that don't sync rotary and linear feedrate.

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

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

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


  7. #7
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Quote Originally Posted by daniellyall View Post
    It's more I just needed to know if G54 was a bad idea at the start and end of the G code for UCCNC yes ger G0 G54 Z0

    The newest UCCNC post for fusion has G53 one of the UCCNC users wonted his changed from G53 to G54 at the start and end.

    I will let him know that have G54 could cause a crash and where it goes its up to him to test it.

    mactec54 the chunk of G Code I posted is not the header from the UCCNC post it just has G90 in it, that was what I had open at the time I posted here.

    I know what G93, G94 and G95 are for
    Well I replied to what you had posted, you gave 2 examples , I gave you what needs to be done to correct your Post processor

    Read the UNCNC Manual it will tell you the same as what I have Posted

    Snips below are from the UCCNC manual

    Attached Thumbnails Attached Thumbnails UCCNC G53 or G54-using-g53-jpg   UCCNC G53 or G54-using-tool-offsets-g54-etc-jpg  
    Mactec54


  8. #8
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Quote Originally Posted by ger21 View Post
    Rotary axis work using G93 makes it easy to get the proper feedrates on the rotary axis moves on controls that don't sync rotary and linear feedrate.
    This would help when you have 4 and 5 axes, but most good Cam program have moved past using a G93 as there are more efficient methods for doing the same thing, there are some 3rd party programs that offer the use of G93

    Mactec54


  9. #9
    Registered
    Join Date
    Feb 2018
    Location
    New Zealand
    Posts
    20
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Quote Originally Posted by ger21 View Post
    [snip]
    Do you mean G0 G53 Z0?
    Personally, I remove that from my post. I don't want the machine to rapid all the way up at the start of my code.
    [snip]
    Sorry Hijack.

    I have just spent a while in the last couple of days trying to find out if that was normal... I have been manually editing out the G0 G53 Z0 from the start (and end) of the F360 produced Gcode and I'm glad it's not just me that found it strange.

    Is there an option in F360 to suppress this, or I guess is there an option to edit the F30 Cam definition to remove it?

    It's not the end of the world to have to remember to take it out manually, and I do have a Z limit switch, but it is annoying.

    Cheers - N



  10. #10
    Member
    Join Date
    Jun 2015
    Location
    Sweden
    Posts
    943
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Quote Originally Posted by Talkiet View Post
    Sorry Hijack.

    I have just spent a while in the last couple of days trying to find out if that was normal... I have been manually editing out the G0 G53 Z0 from the start (and end) of the F360 produced Gcode and I'm glad it's not just me that found it strange.

    Is there an option in F360 to suppress this, or I guess is there an option to edit the F30 Cam definition to remove it?

    It's not the end of the world to have to remember to take it out manually, and I do have a Z limit switch, but it is annoying.

    Cheers - N
    I'm not using Fusion, but the code which outputs that G53 should be in the post processor.
    Try to check the post processor file and find where it posts that piece of code.
    Or ask Autodesk customer or tech support about it.



  11. #11
    Gold Member daniellyall's Avatar
    Join Date
    Sep 2009
    Location
    New Zealand
    Posts
    1856
    Downloads
    3
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Talkiet That is a simple edit I do that one all the time, I usely have it so it is a G53/G28 or a set position what is just a yes no selection to change it or G53/G28 and a nothing.

    I can do it for you or just tale you, You just have to make sure that the post is keeped up to date with the code changes, they are slow make it so a post edit is simple as mud useing the Visual studio editor they have done and have a end or start code different to in the G code it self.

    Whats is a pain haveing to redo posts each big update of the CAM.

    <img src="https://ivxo1q-dm2305.files.1drv.com/y4mENMmTr_Cabc7pR0FUdB6gtbADq2JbuG4_rGy0eBQvLJx19pTi6TqMUIJN0xgOyDIc0gWoxYhS38HpbSTFGdfaK-o42IOU6jczrhDpfpCOTNGL1X6hvZCbgj0y35gqmq1YGTrWwShYGV-C7lXA2esy0Pi_WfnBSyroDLSGXwce4uSr1U7op7srdi78rispHCa_K4aFlTlJPVkkNWMfgh_Tg?width=60&height=60&cropmode=none" width="60" height="60" />

    Being Disabled is OK CNC is For fuN


  12. #12
    Registered
    Join Date
    Feb 2018
    Location
    New Zealand
    Posts
    20
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    I'm comfortable coding etc so I'll have a look around first before asking for specific assistance - just knowing that I need to edit the post proc file is the hint I need.

    I also need to modify the 2017 screenset to include the homing offsets - although I can manually put the parameters into the profile config, and they are loaded and used fine, the screenset overwrites them with zeros when I save it again...

    I guess it's time to break out notepad++

    Cheers - N



  13. #13
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: UCCNC G53 or G54

    I also need to modify the 2017 screenset to include the homing offsets
    Do you mean the homing backoff distances from the test versions? Just use the screen editor to add the fields somewhere.

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

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

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


  14. #14
    Registered
    Join Date
    Feb 2018
    Location
    New Zealand
    Posts
    20
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Sorry, yes, I mean precisely the homing backoff distancesfrom the test versions. I just checked and they solve my prox sensor getting stuck in limits after homing perfectly.

    (The offsets that are in the production versions don't help)

    Cheers - N



  15. #15
    Registered
    Join Date
    Feb 2018
    Location
    New Zealand
    Posts
    20
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Thanks for the suggestion Gerry - I added the X/y/z homing backoffs tonight and it works perfectly with the screenset.

    Cheers - N



  16. #16
    Member
    Join Date
    Jun 2015
    Location
    Sweden
    Posts
    943
    Downloads
    0
    Uploads
    0

    Default Re: UCCNC G53 or G54

    Quote Originally Posted by Talkiet View Post
    Sorry, yes, I mean precisely the homing backoff distancesfrom the test versions. I just checked and they solve my prox sensor getting stuck in limits after homing perfectly.

    (The offsets that are in the production versions don't help)

    Cheers - N
    The offset is the home coordinate it does not back the axis off is why it does not help for your problem.



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

UCCNC G53 or G54

UCCNC G53 or G54