Peck drilling problem with Siemens 840D controller

O

Owl Engineering

Plastic

Joined

Nov 13, 2005

Location

Warren, Michigan USA

• Sep 19, 2008

• #1

Any ideas how to program peck drilling after a starter hole?

Example: If I drill 1" deep with a short screw machine drill and now want to finish the hole 2" deep with a standard length drill, how can I program so that the long drill rapids down to the 1" point, drills .10 and rapids out to 0.0 for chip removal and than rapids back down to the -1.1 point etc.?

Thank you in advance, Chuck

 

D

Dave K

Diamond

Joined

Mar 21, 2004

Location

Waukesha, WI

• Sep 19, 2008

• #2

Are we talking about straight G code programming, or are we talking about shopmill programming?

 

O

Owl Engineering

Plastic

Joined

Nov 13, 2005

Location

Warren, Michigan USA

• Sep 22, 2008

• #3

Type of program G83

The code that I am using is: Go 83 like this: (.10,.0,.10,-1.00,,.3,,.125,,,1.,1)
The above code is for the first drilling. 1.00 total depth, .3 first depth and .125 deeper each peck.

If I do this: (.10,-1.00,.10,-1.00,,.3,,.125,,,1.,1) it will rapid down but not retract to the top ( 0.00 ) of the part.

Thanks, Chuck

 

D

Dave K

Diamond

Joined

Mar 21, 2004

Location

Waukesha, WI

• Sep 22, 2008

• #4

Chuck from Detroit said:

The code that I am using is: Go 83 like this: (.10,.0,.10,-1.00,,.3,,.125,,,1.,1)
The above code is for the first drilling. 1.00 total depth, .3 first depth and .125 deeper each peck.

If I do this: (.10,-1.00,.10,-1.00,,.3,,.125,,,1.,1) it will rapid down but not retract to the top ( 0.00 ) of the part.

Thanks, Chuck

Click to expand...

Sorry Chuck, I'm not used to using the G83 command on the siemens. I use the shopmill side of the control. As far as I know, that G83 line should look like this:

G83 G99 R.1 Z-1.0 Q.1 F10.

Just for example, the Q.1 makes it peck every .1 depth. The feed rate is 10. inches per minute, comming from the F10. You're final Z depth is 1.0 deep named by the Z-1.0.

That's fanuc style programming, and I thought the seimens used the same but maybe not. Hope this helps.

 

3

3t3d

Diamond

Joined

Nov 1, 2004

Location

WI

• Sep 22, 2008

• #5

It is not a question of Fanuc vs Siemens programing....
It is, How do I start the peck cycle deeper than the R Plane?

The OP wants to keep the R plane above the part for chip clearance, but the pre-drill hle is deeper than the R plane.

I don't think that the Fanuc programming example will help. I think he Knows how to program the standard peck drill cycle, but need a different version of it.

I'm not familiar with the Siemens, In myFanuc I'd (AFIK) have to write a macro program to do it. On My A2100's they already have a cycle to do such a thing.. (IIRC)

 

D

Dave K

Diamond

Joined

Mar 21, 2004

Location

Waukesha, WI

• Sep 22, 2008

• #6

Yeah, you're right. I lost track of the original question. Sorry. I'm of no help here, Chuck.

I know how to do this in the shopmill side, but not the g-code side.

 

rklopp

Diamond

Joined

Feb 27, 2001

Location

Redwood City, CA USA

• Sep 22, 2008

• #7

Can't you do this in G83 by tweaking the lift-off per peck and safety plane parameters? I think you can on Deckel Dialog G-code (ca. 1986). Usually the lift-off per peck is only 0.002" for example, but it might work if you set the lift-off to 1.1" or some similarly huge distance. I'll have to try it some time. :-)

 

O

Owl Engineering

Plastic

Joined

Nov 13, 2005

Location

Warren, Michigan USA

• Sep 23, 2008

• #8

I kind of goofed with my question, explaination

Actually I am using ShopCam programming, a custom post processor and dumping it into the Siemens 840D so I guess the question is how to program using G codes? Or what ever ideas you have.
Thanks for all your efforts so far on this one. Chuck

 

L

Lanza

Aluminum

Joined

Jun 22, 2007

Location

Western Australia

• Sep 23, 2008

• #9

If you were only doing a couple of holes, could just start the R point above the surface of the job, means you will be drilling air for 1".
If you dont know how to make your own canned cycles up. You could manual progarm a series of canned cycles (G81 is normal spot drill on the machines i use) using a increase ments in Z depth and increasement R- value each canned cycle. Put these in a subprogram, if you have a series of holes.
The proper way would be to make you own canned cycle or something with macros.

 

T

Tonytn36

Diamond

Joined

Dec 23, 2007

Location

Southeastern US

• Sep 23, 2008

• #10

Something along these lines may help. Someone double check my logic, it's been a very long, stressful day.


(ALL VALUES TO BE INPUT AS POSITIVE NUMBERS - ASSUMES THAT Z0 IS STARTING POINT)
R200 = 0 (INITIAL DEPTH)
R201 = 0 (PECK DEPTH)
R203 = 0 (RETRACT HEIGHT - R PLANE)
R204 = 0 (TOTAL HOLE DEPTH)
R205 = 0 (SAFETY PLANE - CLEARANCE ABOVE R PLANE)
R206 = 0 (FEED RATE FOR DRILLING)
R210 = 0 (DISTANCE TO STOP ABOVE START OF DRILLING)
(CALCULATIONS AND CODE BELOW)
R207 = 0 (INITIAL COUNT)
R208 = (R204-R200)/R201 (NUMBER OF PECKS REQUIRED - PECK COUNT)
WHILE R207 < R208
G0 Z=-(R200+((R207*R201)-R210))
G1 Z=-(R200+(R201*R207)) F=R206
G0 Z=0+R203
R207 = R207+1
ENDWHILE
G0 Z=0+R205
M17

 

A

Andrej Čulk

Plastic

Joined

Sep 18, 2021

• Sep 18, 2021

• #11

Is a simmilar topic, i hawe the same problem with holes on controller "840D" with "shopmill". Maybe it is possibly do that with standard cycles, or it is only way creating own cycle, e.g. "CYCLE83_3"? In the "CYCLE 83_3" i would add an additional parameter. This parameter will specify another different high of retraction plane.

It is possible this only with R-parameters, like in post above from "Tonytn36", or it is possible also with print in parantheses, as for standard cycles?