Post Processor Mod


Results 1 to 12 of 12

Thread: Post Processor Mod

  1. #1
    Registered bcavender's Avatar
    Join Date
    Apr 2016
    Location
    United States
    Posts
    59
    Downloads
    0
    Uploads
    0

    Default Post Processor Mod

    Dan,

    My target machine is an Okuma 4020 VMC.

    I made a simple Rhino model to gen a test post to compare to another known workable post. After digging deep into both there were only two points that appear to come close in needing attention:

    First, most of the current posts I have seen going to the Okuma use Inches Per Revolution with a specific G95 call up front. The ISO_G_Code.txt (attached) feeds are in Inches per Minute, but don't have a specific G94 code up front. Possibly G94 (IPM) is the default for this machine, but I would really like to get that specific code automatically in the generated as a point of safety as I want to make 100% absolutely sure that there is never a misinterpretation that the feed rate would be 30 Inches per Revolution. (saw that happen before with a FCAM bug-def not pretty).

    Second, I would like to have the spindle home at the end of the post just before the M30. The command I would like to insert is G30P32.

    I read through the ISO_G_Code.txt file to try to get a clue as to how these inserts might be done, but that didn't help me.

    I am at ground zero for learning how to modify Post Processors for madCAM.

    Can you point me to a resource where I can jump start my understanding for how to make these two mods or an example of how this is done so I can start up the learning curve and get out to the machine?

    Thank you!

    Best regards,

    Bruce

    Similar Threads:
    Attached Files Attached Files


  2. #2
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Hi Bruce,

    I can do this for you right now. Just one question: What does your G94 line need to look like? Is it simply G94 you are looking for in the safety line? Like this: G40 G54 G80 G90 G94?

    Also, I see you enabled fixture offsets, but you don't have it set in the post. I'll fix that too.

    Be aware that there is more control available than you currently are seeing in that post you attached. For example, you can control the first move (not to be confused with First Cut). Here is what mine looks like for our Doosan:

    *FIRST_MOVE*
    N"lnbr" G00G90"fixture_offset""x""y"S"speed"M3
    N"lnbr" G43H"toolnr"D"toolnr""z""coolant_on"
    N"lnbr" M24
    N"lnbr" G05.1Q1R10
    N"lnbr" G00"cutter_comp""x""y"
    N"lnbr" G00"z"
    *END_SECTION*

    Here is another section you could add for when the next path doesn't need a tool change. In the following example I just add a note in the post so the operator knows where the paths start and end (since there is no toolchange to indicate this):

    *TOOLPATH_CHANGE*
    N"lnbr" ( TOOL "toolnr" CONTINUES)
    *END_SECTION*

    Anyway, let me know about that G94 and I'll repost the altered post.

    Thanks,

    Dan

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


  3. #3
    Registered bcavender's Avatar
    Join Date
    Apr 2016
    Location
    United States
    Posts
    59
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Dan,
    Thanks for the reply.

    Here is the line I believe you are looking for ... from a FeatureCAM post that works with the Okuma.

    -----------------------------------------------------------------------
    $Oct26a.MIN%
    ( FEATURECAM POST FOR OKUMA MILL WITH OSPU10M CONTROL )
    ( OUTPUT IN ABSOLUTE INCHES 9-30-2017 )
    CLEAR
    DRAW
    NT1 G0 Z20 G17 G40 G80 G95
    N40 G111 T1 Q2
    N45 M1
    ( OPERATION - FINISH FACE ON FACE1 )
    ( TOOL NO - 1 DIAM - 0.496 )
    -------------------------------------------------------------------------

    G40 is there.
    G54 looks good ... as I assume with no arguments the X tool length offset = 0
    G80 is there
    G90 looks good for absolute mode
    G94 for Inches per Minute


    In studying it a little further, I think I am beginning to see how it is working with madCAM. It appears that the 'post processor' text file is essentially a mini-database of *ACTION* keys that designate a data record of a G-code format (with variables) that should be generated for the specific target machine. During the post processing cycle, the CAM package searches through the table for a certain *ACTION*, picks up the associated data structure for that action and then creates a G-code string that fits the target machine and writes it to a file. Is that close?

    THANKS!!!

    Bruce



  4. #4
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Yeah, that sounds about right. Here is the post. See if it works as expected.

    Dan

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


  5. #5
    Registered bcavender's Avatar
    Join Date
    Apr 2016
    Location
    United States
    Posts
    59
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Dan,

    Great! Thank you! Seeing the changes make sense. That helps the learning process immensely. It is not a complex as it first seemed. The changes you entered worked posted out perfectly.


    In trying to make sure the physical Okuma parameters are on beam with what is in this file I have these last questions about definitions and units:

    *FILTER* - 0.001 What is being filtered here?

    *Output Width* - 4 What is this width?

    *Rapid Feed* - 10000 Inches per minute?

    *ToolChange Time* - 0.3 Units in seconds?

    *Line_Start_Number* - 0
    (The post output doesn't contain line numbers ... I tried changing the start number to 5 to see if that would enable line numbering, but it did not.
    How can I enable line numbers?

    Appreciate your good help!!!

    Bruce



  6. #6
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Hi Bruce,

    The Filter has to do with tolerances in the toolpath. I believe by setting a value, it ignores values below what you set. In other words, if I set it to .001 than any move that's smaller. like .0005 will not force extra code to be produced.

    Output width seems to be a bit of a mystery. I've tried to change that setting just to see what it does and I've never seen any difference in the code. I just leave it alone and there are no issues.

    The Rapid Feed is going to be in the units that your post is set to. For example, if you have G20 in your code you are working in imperial. G21 is metric. I've never worked in imperial, so I've never explored what happens when you do, but I don't recall anywhere other than the post where I have to specify the units being used. If you don't specify a G20 or G21 (could be G70 and G71 on older controllers) then the controller configuration will be used. If your controller is set to inches, and you feed what you intended to be a metric program without a G21, you are going to slam into your stops immediately. Anyway, that Rapid Feed setting has no affect on the output code. It's used for time calculations only.

    The ToolChange Time is also just for reporting and has no effect on the output code. It is a fraction of a minute. So if your machine can do a toolchange in 15 seconds, you would put .25 there. If it takes 30 seconds, then enter .5, etc.

    If you want line numbers you need to add N"lnbr" to the start of the lines. You can see that in the samples I posted above.

    Hope this helps,

    Dan

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


  7. #7
    Registered bcavender's Avatar
    Join Date
    Apr 2016
    Location
    United States
    Posts
    59
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Dan,

    I fine tuned the Filter and got LineNumbers working. The post I generated with the new file looked good. I will give it a run on the machine tomorrow.

    Question:

    The Okuma has the ability to do Circular Interpolation G02/G03.

    Can I add these commands to my post processor table to give madCAM access to these commands (if madCAM has this internal capability)?

    THANK YOU!

    Best regards,

    Bruce



  8. #8
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Hi Bruce,

    Yes you can:

    *CW_ARC_MOTION* //Characters to set for the "motion" variable. For example: G02

    *CCW_ARC_MOTION* //Characters to set for the "motion" variable. For example: G03

    *ARC_RADIUS_CHAR* //Output character for arc radius.

    *ARC_DX_CHAR* //Output character for the arc center X-offset. (arc center - arc startpoint).

    *ARC_DY_CHAR* //Output character for the arc center Y-offset. (arc center - arc startpoint).

    *ARC_DZ_CHAR* //Output character for the arc center Z-offset. (arc center - arc startpoint).

    Unfortunately I don't have an example of these post commands utilized in a working post. But it's definitely possible.

    Dan

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


  9. #9
    Member
    Join Date
    Feb 2006
    Location
    Sweden
    Posts
    183
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Hi Bruce,

    There is a variable "motion" that can be defined as linear, arc clockwise or arc counterclockwise. (See below).

    *ARC_RADIUS_CHAR*
    R

    *RAPID_MOTION*
    G00

    *LINEAR_MOTION*
    G01

    *CW_ARC_MOTION*
    G02

    *CCW_ARC_MOTION*
    G03

    You can then use these by typing "motion" in each section.
    :
    :
    *FIRST_CUT*
    "motion" "x" "y" "z" "r" F"feed"
    *END_SECTION*

    *CUT*
    "motion" "x" "y" "z" "r"
    *END_SECTION*
    :
    :

    It is also possible to include coordinate variables when defining each motion.

    *PLANE_XY*
    G17
    *PLANE_XZ*
    G18
    *PLANE_YZ*
    G19
    *ARC_RADIUS_CHAR*
    R

    *RAPID_MOTION*
    G00 "x" "y" "z"
    *LINEAR_MOTION*
    G01 "x" "y" "z"
    *CW_ARC_MOTION*
    "plane" G02 "x" "y" "z" "r"
    *CCW_ARC_MOTION*
    "plane" G03 "x" "y" "z" "r"

    When the coordinate variables are included with each section, it's enough tu just type "motion" in each section.

    *FIRST_CUT*
    "motion" F"feed"
    *END_SECTION*

    *CUT*
    "motion"
    *END_SECTION*



    I hope this will give you some help.

    /Joakim



  10. #10
    Member
    Join Date
    Feb 2006
    Location
    Sweden
    Posts
    183
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Below is a sample post processor.

    //MadCAM_POST_2014-01-22
    *VERSION*
    5.0_131211
    *FILE_NAME*
    Gcodes with arcs
    *FILE_EXTENSION*
    txt
    *FILE_DEST*
    c:\postfiles\
    *FILTER*
    0.005
    *OUTPUT_WIDTH*
    0
    *OUTPUT_DECIMALS*
    3
    *SCALE_X*
    1
    *SCALE_Y*
    1
    *SCALE_Z*
    1
    *AXIS_1_CHAR*
    X
    *AXIS_2_CHAR*
    Y
    *AXIS_3_CHAR*
    Z
    *PLANE_XY*
    G17
    *PLANE_XZ*
    G18
    *PLANE_YZ*
    G19
    *ARC_RADIUS_CHAR*
    R
    *ARC_DX_CHAR*
    I
    *ARC_DY_CHAR*
    J
    *ARC_DZ_CHAR*
    K
    *ARC_CW_CHAR*
    R
    *ARC_CCW_CHAR*
    R-
    *RAPID_MOTION*
    G00 "x" "y" "z"
    *LINEAR_MOTION*
    G01 "x" "y" "z"
    *CW_ARC_MOTION*
    "plane" G02 "x" "y" "z" "r"
    *CCW_ARC_MOTION*
    "plane" G03 "x" "y" "z" "r"
    *CUTTER_REFERENCE*
    TIP

    *FIRST_MOVE*
    (First move---------------)
    "plane"
    "motion"
    (---------------First move)
    *END_SECTION*

    *RAPID*
    "motion" (---------------Rapid)
    *END_SECTION*

    *RAPID_APPROACH*
    "motion" (---------------Rapid Approach)
    *END_SECTION*

    *RAPID_RETRACT*
    "motion" (---------------Rapid Retract)
    *END_SECTION*

    *APPROACH*
    "motion" F"feedz" (---------------Approach)
    *END_SECTION*

    *FIRST_CUT*
    "motion" F"feed" (-------------First cut)
    *END_SECTION*

    *CUT*
    "motion" (-----------------------------Cut)
    *END_SECTION*

    *LAST_CUT*
    "motion" (------------------------Last cut)
    *END_SECTION*

    *TOOL_CHANGE*
    ("toolname")
    M6 T"toolnr"
    M03 S"speed"
    *END_SECTION*

    *TOOL_STOP*
    (Tool Stop)
    G40
    M5 M9
    (-------------Tool Stop)
    *END_SECTION*

    *PROGRAM_START*
    G00 G49 G40 G80 G50 G90 G64
    *END_SECTION*

    *PROGRAM_END*
    M30
    *END_SECTION*

    *LINE_START_NUMBER*
    1



    /Joakim

    Attached Files Attached Files


  11. #11
    Member
    Join Date
    Feb 2006
    Location
    Sweden
    Posts
    183
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    I forgot to mention that the arc support is only for the 2D Profiling function at the moment. The new 2D Profiling is generating nurbs as toolpaths. The curves will be converted to arcs when post processing (If choosing that from the options dialog). If the nurbs curve includes arcs, the conversion is exact.

    /Joakim



  12. #12
    Registered bcavender's Avatar
    Join Date
    Apr 2016
    Location
    United States
    Posts
    59
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor Mod

    Dan/Joakim,

    Thank you for the info on circular interpolation. I will have to dig into that when I can get some quiet time to come up to speed. That's next on my list.

    I ran six test posts today on the Okuma that were simple to progressively more complex to try to wade in carefully and build confidence in what I am doing.

    Every post ran perfectly with the modified ISO post processor.



    That's good progress for me with only a week under the belt starting from absolute zero knowledge about post processors.

    Can't wait to dig in further.

    Really appreciate your guys knowledge and help!

    Great product!

    Thanks!

    Bruce

    Attached Thumbnails Attached Thumbnails Post Processor Mod-blockpic-jpg   Post Processor Mod-ok-jpg  


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

Post Processor Mod

Post Processor Mod