First Time CnC, Contour 3 help needed!
Close
Login to Your Account
Page 1 of 4 123 ... LastLast
Results 1 to 20 of 75
  1. #1
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    35

    Default First Time CnC, Contour 3 help needed!

    Hello!

    I have never used a cnc machine before. I am trying to learn the basics.

    I have tried to program with a sharpie marker some g2/3 codes. I can make full circle and 180' etc. But when i try to add a straight cut before a 180' turn i get error 95 all the Time. The g2/3 code Works without a g91 straight cut block.

    Can someone give me an example of the program structure, what is needed to a complete program.?

    I see some examples over the internet with 2 different g codes in same block, how i can do this?

    I appreciate all help what i get here, i am total beginner with these and got no one to teach me.

  2. #2
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    754
    Post Thanks / Like
    Likes (Given)
    1043
    Likes (Received)
    176

    Default

    Post the code you are trying to run and we can help troubleshoot it

  3. #3
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    35

    Default

    The machine is a 1hour drive away from me, cant remember the whole code. But if i had a working block with g2/3 code and i added a g01 or 91 with short x axis cycle before it i had error 95.

    Can someone show how to write a complete code with all command needed to shape in link.

    oval curve shape - Google Search

  4. #4
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    754
    Post Thanks / Like
    Likes (Given)
    1043
    Likes (Received)
    176

    Default

    Quote Originally Posted by Harri89 View Post
    The machine is a 1hour drive away from me, cant remember the whole code. But if i had a working block with g2/3 code and i added a g01 or 91 with short x axis cycle before it i had error 95.

    Can someone show how to write a complete code with all command needed to shape in link.

    oval curve shape - Google Search
    If you can't remember or post the code, how can you expect anyone else to know how you've set up the program and where you are having problems?
    Are you trying to machine the inside of that oval, or the outside? Are you using tool compensation or not? Makes a big difference in how the program is written.Does your control have the "parameter" option?

  5. Likes Fancuku liked this post
  6. #5
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    35

    Default

    No tool compensation, the oval line is just the center of "tool"
    I am just trying to understand the structure of program, what is needed.

    Zero point left front corner.
    R is 15mm trying to do 180' so p1 and p2 in arc distance 30mm

    It was something like this..

    N1 g00 x20 y20 z1 s100
    N2 s100 f100 z0
    N3 g91 x20 s100 f500
    N4 G3 x40 y50 i0 j15

    I am trying to learn tool paths, not easy to start from nothing :/
    Last edited by Harri89; 12-02-2018 at 01:24 AM.

  7. #6
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    754
    Post Thanks / Like
    Likes (Given)
    1043
    Likes (Received)
    176

    Default

    Try this:

    N1 S+1000 F100 Z25
    N2 G0 X0 Y0
    N3 Z0
    N4 X50
    N5 G3 X50 Y30 I0 J15
    N6 X0
    N7 G3 X0 Y0 I0 J-15
    N8 G0 Z25
    N9 M30

  8. #7
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    754
    Post Thanks / Like
    Likes (Given)
    1043
    Likes (Received)
    176

    Default

    Could also be done like this:
    N1 S+1000 F100 Z25
    N2 G0 X0 Y0
    N3 Z0
    N4 G2 X0 Y30 I0 J15
    N5 X50
    N6 G2 X50 Y0 I0 J-15
    N7 X0
    N8 G0 Z25
    N9 M30

  9. #8
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    35

    Default

    If i understand right, i need to add spindle speed and feed speed to each block separately where is a feed motion done? Rapids doesnt need them necessarily?

  10. #9
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    754
    Post Thanks / Like
    Likes (Given)
    1043
    Likes (Received)
    176

    Default

    Quote Originally Posted by Harri89 View Post
    If i understand right, i need to add spindle speed and feed speed to each block separately where is a feed motion done? Rapids doesnt need them necessarily?
    Spindle speed and feed are what is called "modal"- they stay active until another G code in the same group is programmed, you only need to put them in once.
    Rapids are done with a "G0" command and on Dialog controls the command is "non modal", it is only activated during the execution of the block to which it is written. (other controls do this differently).

    Check out this video, it might help you with general concepts Deckel NC Milling Made Easy - YouTube

  11. #10
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    35

    Default

    Good video! Thank you for it
    I ordered today a nc book to study, maybe i'll get it next week

    Is there somewhere made an list of all commands for dialog controls?

  12. #11
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    754
    Post Thanks / Like
    Likes (Given)
    1043
    Likes (Received)
    176

    Default

    There should be an "orange book" that goes with your machine and has programming information in it.
    On the right side of the operator console, next to the keypad, there should be a flip chart (approx 75x125mm in size) that has most commands and error codes in it.

  13. #12
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    35

    Default

    I have that, but its written in German

  14. #13
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,548
    Post Thanks / Like
    Likes (Given)
    2115
    Likes (Received)
    2937

    Default

    Flip cards are pretty graphic...When i first got my FP4NC it had German cards and i was able to get the idea just looking critically at the graphics....

    What you really need is the operators manual for your machine /control....gives lots of programming examples, easy to follow for each of the commands....invaluable.
    Not up to speed as to the exact differences but a Contour3 is roughly equivalent to a Dialog4 control as to programming.

    Some general notes:
    Dialog must have a speed code (S+/S-) programmed in order to allow any feed moves (G01/G02)
    Any called linear move (target point) is assumed by the control to be a feed move, you do not need to have a G01 or G02 programmed in the move code. But you must have previously
    programmed a feed rate ...
    Once a feed rate is programmed it will stay in effect till it is overridden with a different feed rate or a rapid move....Must then recall a feed rate to continue with an linear move....
    If you are doing a drawing using a pen in the spindle and don't wish it to be rotating while running the program "proof" you can use speed code S+0...Control believes the spindle is in motion so the
    program will run, but the spindle will not rotate.
    Rapid moves must be called every time they are needed (in every block where desired)
    Canned cycles almost include a call fro feed rate within the cycle....
    Canned cycles with depth moves use incremental (G91) valuers for all depths within that cycle...even if you are programming in absolute (G90).

    Cutter comp has more "rules" that have to be followed in order for it to function...
    Establish a routine as to how to start every program ! This will simplify the program writing and eliminate errors...
    As example, i always start every program by moving rapid to the tool change point...Somewhere off the part surface and at the datum (zero point) of the program...
    I also set the direction for length comp right off. as well as the spindle speed...
    Example in inches:

    N1 G0 X0.0 Y0.0 Z4.0
    N2 G17 T1
    N3 S+1000
    N4 G0 X1.0 Y2.4 Z.1.
    .................................................


    Block 1 sets the tool change point and moves there.
    Block 2 calls the length comp for a vertical tool and defines the first tool (T1) Must have a tool 1 defined in the tool store (mode 10)
    Block 3 starts the spindle at 1000 RPM rotating to the right (forward)
    Block 4 moves the tool at rapid to a clearance height off the part and at the start point of the cut....Note trailing zeros (to the right of the decimal point) are not needed....But i always write them in my
    paper copy (Manuscript) as i am creating the program....

    Cheers Ross

  15. Likes skippy liked this post
  16. #14
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    35

    Default

    Thank you for your help!! I had success

    Now a new problem, i tried to mill a pin and if i would do this with a tool it would break. I dont know why the "tool" moves through the "pin" To the center?

    Below pic of the g75 code and a video

    Deckel FP4A Testing 3 - YouTube


    img_20181207_124320.jpg

  17. #15
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    754
    Post Thanks / Like
    Likes (Given)
    1043
    Likes (Received)
    176

    Default

    You wrote the program correctly.
    The tool should retract after the last circular pass an all the Z moves have been made. Then the tool should move up in Z (table moves down) to your starting point (Z0 in the previous block), then the tool returns to the XY starting point, which is the center of the pin (X40 Y40).

    Your Z moves are very small so it is probably hard to see the machine move in Z.

    Good job!

  18. #16
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,548
    Post Thanks / Like
    Likes (Given)
    2115
    Likes (Received)
    2937

    Default

    Think you need a clearance plane before you call the G75.

    Something like this:
    N1 G0 X0.0 Y0.0 Z100.0
    N2 G17 T1
    N3 S+0
    N4 G0 X40.0 Y40.0 Z5.0
    N5 G75 F1500 S+0 G3 X40.0 X15 Y20.0 Y.4 F100 Z-5.1 Z-5.1 Z-.050
    N6 G0 Z100
    N7 G0 X0.0 Y0.0
    N8 M30

    The way the cycles work is that the tool returns the the height where the cycle was started once the cycle is complete....
    You started at height 0.0 so the tool did not retract upon completion....
    Remember to add the height of your clearance plane (in my example 5mm) to your depth of cut....
    Also i usually use a down feed increment larger than the required depth if i am going to cut it in one pass for depth...that way if i need to add to the cutter comp in length an re-run the code to get
    the cut deeper i don't need to change the base program...

    Also not sure how the control handles the depth (Z) move if you don't have an increment value...your sample (screen shot) shows zero...never tried it that way....

    Other habits worth considering....When working within a contour or bore I always rapid to the center of the profile before moving up to the tool change point....
    If running on the outside of a contour...do the "Z" up first then rapid to your tool change point (X0.0 Y0.0)....I always make my end of program in three blocks:
    The two to position the tool depending on the profile and the final being the M30 (stop rewind)



    Cheers Ross

  19. Likes Colt45 liked this post
  20. #17
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    35

    Default

    Okay, thanks for the info! Very pleased for your help
    I also tried a subroutine run, that seems to be very useful.

    I am getting closer to running a practice run with an end mill

    Need to try with the clearence plane next time im going to run the machine.

    It will take time to learn how to use the control efficiently. I think it will be good to know how its done programming by hand before transfering it from computer.
    Is there a cam software which Works directly with dialog 4 /contour 3 control or do they always need a postprocessor?

    This is all new to me so my questions may be little stupid

  21. #18
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,548
    Post Thanks / Like
    Likes (Given)
    2115
    Likes (Received)
    2937

    Default

    Think all CAM systems require a post processor...That is how the general program can be tailored to the exact needs of each machine builder....
    Otherwise the cost of making an individual program that was native to your exact machine would be cost prohibitive!

    Deckel did make and provide a stand alone programming station that could solve geometry for intersections and angles etc. Never seen one in person but believe they did exist...Likely by now those would be long dead.

    As to the clearance plane....Something that really should be part of all programming for any cutting moves...Nobody rapids a cutter to the point of beginning the depth cut...
    It just is not wise...slight overshoot and you kill the tool and perhaps the part.
    Cheers Ross

  22. Likes Colt45 liked this post
  23. #19
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,176
    Post Thanks / Like
    Likes (Given)
    216
    Likes (Received)
    1046

    Default

    Quote Originally Posted by Harri89 View Post
    Is there a cam software which Works directly with dialog 4 /contour 3 control or do they always need a postprocessor?
    I am not aware of any CAM that does not need a post-processor, since different controls need different g-code to do the same tool paths. Nowadays, the post processor can be tightly integrated with the CAD/CAM software, and you don't perceive that you are running a separate program.

    I have a post-processor for Fusion 360 that I tweaked for Dialog 4. It's based on one that you can download from Autodesk. Still, you can make better code by hand. Modern posts don't realize that Dialog 4 runs on thirty-year-old computers. Operations like adaptive clearing don't work very well, because the processor chokes on too many moves. The best strategy I have found in Fusion is to use "Smoothing" all the time, and use compensation on the contour (G41/G40) whenever possible. The Dialog pauses a lot less when using G41. Smoothing turns as many curves into arc moves as possible. Otherwise, there are many small straightline moves that choke the control.

  24. Likes AlfaGTA, Colt45, jz79 liked this post
  25. #20
    Join Date
    Nov 2016
    Country
    FINLAND
    Posts
    315
    Post Thanks / Like
    Likes (Given)
    35
    Likes (Received)
    35

    Default

    I need to do a X shape plate with 8 curves to different directions With g2/3 code.

    I am running the "X" cw direction
    Do i need to use g41 every time before g2/3 or does it stay in use before deleting the contour with g40?

    I dont understand the g45, 46 and 47 approaches, how do i use them?


Tags for this Thread

Bookmarks

Posting Permissions

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