Author Topic: drilling  (Read 1568 times)

Offline hana

  • Ewok
  • *
  • Posts: 10
    • View Profile
drilling
« on: January 13, 2020, 11:40:10 am »
Hi, I am very new in cambam nad CNC generally.. Can you help me with small problem, please.. I need to drill approx 1000 deep holes in block. All the same. But when I use peck and retrag, gcode makes it only on the first hole and the rest goes without retracting. How to write it to do it on all block?
thank you!!


Good point, attached the file. Tool 2, depth 20mm. Thank you!!
« Last Edit: January 13, 2020, 13:15:48 pm by hana »

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 2953
    • View Profile
Re: drilling
« Reply #1 on: January 13, 2020, 13:06:01 pm »
If you attach the CB file, that would make lot easier to help you..
My 2ยข

Win 10 64 bit, CB [1.0} rc 1 64 bit, Mach3, ESS, G540

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8314
    • View Profile
Re: drilling
« Reply #2 on: January 13, 2020, 16:54:50 pm »
Hana,
I think you attached the wrong file.  There are no machining operations in the one you attached.

We don't wish to see only the drawing, we wish to see how it's presently being machined, so we may offer corrections.

Yours,
Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline hana

  • Ewok
  • *
  • Posts: 10
    • View Profile
Re: drilling
« Reply #3 on: January 13, 2020, 18:09:28 pm »
OK, I didn't know. I wrote code for simple drilling in this case, but coming another, where is lifting necessary and I don't know how.
Attached what I did only.
thanks for help!!

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8314
    • View Profile
Re: drilling
« Reply #4 on: January 13, 2020, 18:40:17 pm »
Have you actually tried drilling, or are you just looking at the g-code?  I ask, because most machines only need the portions of a drilling cycle that have changed since the last iteration of that cycle.

However, if your machine needs ALL the parameters for every cycle, you'll need to add this clause to your post-processor:   <DrillPeck>G83 {$x} {$y} {$z} {$q} {$f} {$r}</DrillPeck>

In addition, I see you have not actually declared a post-processor.  Load the 'default' PP into a text editor, add that line, then save it to a NEW Name.cbpp (save it in the post-processors directory).

Use that name (without the .cbpp suffix) as your Post Processor name in the Machining tab of your most-recent .cb file, and save the file.

Lloyd
« Last Edit: January 13, 2020, 20:15:30 pm by lloydsp »
"Pyro for Fun and Profit for More Than Fifty Years"

Offline hana

  • Ewok
  • *
  • Posts: 10
    • View Profile
Re: drilling
« Reply #5 on: January 13, 2020, 21:37:05 pm »
Wow! Thank you!!! And yes, actually drilling. New product, 1 piece, not for production, tool for us. Every piece different proces and tool.
Thank you very much for help, started a month ago, still learning a lot...

Online dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6058
    • View Profile
    • Cambam V1.0 French Doc
Re: drilling
« Reply #6 on: January 13, 2020, 23:41:27 pm »
Hello

Peek drilling needs that you set a value for "Peck Distance" ; if not, there is no peek.

Note also that simulator like cutviewer show only the peek for the first hole, not for others (but there are done on the machine)

"Retract Height" can be set to the same value as stock surface to speed up things.

++
David


Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8314
    • View Profile
Re: drilling
« Reply #7 on: January 13, 2020, 23:51:13 pm »
Yes!  You must declare a 'peck distance'.  I had typed that in my previous response, and somehow deleted it before posting.

Not only is the <DrillPeck>...</Drillpeck> clause necessary, but you MUST declare a peck distance in the drilling MOps.

Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline Garyhlucas

  • CNC Jedi
  • *****
  • Posts: 1368
    • View Profile
Re: drilling
« Reply #8 on: January 14, 2020, 03:18:45 am »
On most machines 70 and 80 cycles are called "modal" meaning they stay in effect until canceled by a G80 call.  So you can set up a drill cycle and then each time the machine moves in X or Y it will repeat at the next location. Note that is even possible to change say the depth after some holes are drilled and set it back again just by calling a new Z depth between X or Y moves.

I used to code all my X&Y moves in a subroutine.  Call a G81 to drill a pilot hole, then the subroutine, call a G83 to drill with a tap drill, then the subroutine, set up the tap cycle and call the subroutine.  Hit the hole locations with the pilot drill and all the others hit correctly as well.
Gary H. Lucas

Have you read my blog?
 http://a-little-business.blogspot.com/

Offline hana

  • Ewok
  • *
  • Posts: 10
    • View Profile
Re: drilling
« Reply #9 on: January 14, 2020, 13:22:08 pm »
thank you very much!! I did set up peck distance and retract, but simulator showed only the first hole. And I had no idea, it could not show it all .....

Lloyd, I did exactly gcode upon your instructions (set peck distance) and it works!!!!  :D I was so proud about myself, jumping here yesterday  ;D Big help, thanks!!

I would like to ask you another problem I have with Mach3. Where in the settings I can slow down G0 movement? It is very very fast, motors are noisy and sometimes even loosing positions.

Offline EddyCurrent

  • CNC Jedi
  • *****
  • Posts: 4409
    • View Profile
Re: drilling
« Reply #10 on: January 14, 2020, 14:37:04 pm »
I would like to ask you another problem I have with Mach3. Where in the settings I can slow down G0 movement? It is very very fast, motors are noisy and sometimes even loosing positions.

In the Motor Tuning page, from Mach3 top menu, Config->Motor Tuning
Change values for "Velocity" and "Acceleration"

Here's a video.
https://www.youtube.com/watch?v=FntKMPw7lZE

It would be a good idea to seach for information on finding the best settings for these values, it varies between machines as you would expect.

« Last Edit: January 14, 2020, 14:41:37 pm by EddyCurrent »
Made in England

Offline hana

  • Ewok
  • *
  • Posts: 10
    • View Profile
Re: drilling
« Reply #11 on: January 14, 2020, 15:08:08 pm »
Quote
In the Motor Tuning page, from Mach3 top menu, Config->Motor Tuning
Change values for "Velocity" and "Acceleration"

That is what I thought, but I cannot rewrite the numbers. After "save axis setting" it jumps back to before numbers. I guess stg is wrong and I should reinstall Mach :(
For the correct numbers I expect that manufacturer should know.

Thanks for advice!!

Online dh42

  • Administrator
  • CNC Jedi
  • *****
  • Posts: 6058
    • View Profile
    • Cambam V1.0 French Doc
Re: drilling
« Reply #12 on: January 14, 2020, 15:15:04 pm »
Hello

Most of the time in Mach3 you must hit the Enter key to validate the value that has been entered in a box.

++
David

Offline hana

  • Ewok
  • *
  • Posts: 10
    • View Profile
Re: drilling
« Reply #13 on: January 14, 2020, 17:23:35 pm »
Still not able to change number of velocity. Even hitting enter. It drops to 0 and cannot change it anywhere else after. Any idea? If I install Mach again, takes origin numbers and these are to high again.

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8314
    • View Profile
Re: drilling
« Reply #14 on: January 14, 2020, 18:12:50 pm »
"Lloyd, I did exactly gcode upon your instructions (set peck distance) and it works!!!!  Cheesy I was so proud about myself, jumping here yesterday  Grin Big help, thanks!!"
------------------

Hey!  Terrific Hana!  I was just the first guy to jump in with a suggestion.  You'll find this to be the MOST helpful technical site on the internet.  In fact, I'm seldom the person who offers a suggestion, because so many people help.

Lloyd
"Pyro for Fun and Profit for More Than Fifty Years"