Printable View
Does anyone know of a way to adjust rapid speeds in code? Right now I have long drills in a peck cycle and I need the rapids turned down for just a few tools. My solution is a M00 and having the operator turn the override to 25% and then another M00 to turn the rapids back to 100% after these tools run. This works great except for when my operator isn't standing right next to the machine.
I would change rapids from G00 to G01 and set the feed wanted.
Hub
In a G83 drilling cycle? How?
You might be able to G10 the parameter. What control do you have?
As others have said change any G0 moves to a G1 with a Feed number of how fast you want to moveQuote:
Originally Posted by MudNation
It would be best if you posted your program, you usually control a G83 with a F--. you may be missing some code
Hardym1
A G10 has nothing to do with Rapids or Feed Rate, it is only used for Coordinate system
The F in G83 controls the rate at which I drill. Not the rate at which I exit the hole. I'm not missing any code. I'm trying to do something unconventional with out having to write my own can cycle. I want to adjust the rapid limit in my code so my operators don't have to for a few tools. I'll post my code tomorrow.
Thanks for the responses.
Here is the section of my code.
N229M00
(SET-RAPID-TO-25-PERCENT)
(1/4-DRILL-LONG)
N230T#109
N231#2001=-4.427
N232G90G00B270.
N233G90G00X5.56Y-1.1S500M03
G43H01Z0
N234Z-4.3M08
N235G01Z-4.6F20.
N236S1000
N237G98G83Z-9.5R-4.5Q.3F4.
N238S500
N239G00Z-4.3
N240X5.07Y-4.44
N241G01Z-4.6F20.
N242S1000
N243G98G83Z-11.77R-4.6Q.3F4.
N244S500
N245G00Z-4.3
N246X7.45Y-4.51
N247G01Z-4.6F20.
N248S1000
N249G98G83Z-8.64R-4.6Q.3F4.
N250S500
N251G00Z0
N252B90.
N253X-5.56Y-1.1
N254Z-4.3
N255G01Z-5.4F20.
N256S1000
N257G98G83Z-9.5R-5.4Q.3F4.
N258S500
N259G00Z0M09
N260#2001=0
N261G28Y0Z0M05
N262M00
MudNation
The only way you will be able to do what you want, is by writing a Macro, it would still call the G83 but do what is written in the Macro, if your control can not use a Macro, then you can only do what you are already doing
Your program is not very well formated, what control does your machine have
My control is an M11. I figured my only option was to write my own macro. I was hoping there would be parameters for rapid limits that I could adjust on the fly.
Thanks mactec54 I appreciate your help.
As others have said change any G0 moves to a G1 with a Feed number of how fast you want to move
It would be best if you posted your program, you usually control a G83 with a F--. you may be missing some code
Hardym1
A G10 has nothing to do with Rapids or Feed Rate, it is only used for Coordinate system .
mactec54
You are wrong that it is only used for coordinate system. I G10 my parameters all the time.
I have used it on fanuc 18, fanuc 21, and fanuc 31 controls. I have made sub programs for setting my feed rates.
:8001(Z RAPID FEEDRATE-25 PERCENT)
G10L50
N1420P3R6000
G11
M99
:8002(Z RAPID FEEDRATE-100 PERCENT)
G10L50
N1420P3R24000
G11
M99
:8003(XY 25 PERCENT)
G10L50
N1420P1R8000
N1420P2R8000
G11
M99
:8004(XY 100 PERCENT)
G10L50
N1420P1R32000
N1420P2R32000
G11
M99
Hardym1
It was not wrong at all not all controls can use it that way, most can not use the Parameter change, but he could try it to see if his control will run it, That is why I also asked MudNation what control he was using
On Fanuc controls a G10 L50 statement can often be used for changing parameters. Sometimes a parameter may be changed while the program is running to inhibit an area by changing the overtravels, or maybe change a parameter that in one part of the program needs to be one way and in another section may need to be the other. A G10 parameter change statement is also sometimes used in probing routines or more commonly to load values into work coordinates or tool offsets.
There are to types of parameters that require two different formats for using G10. One is used when there is 8 separate bits within the one parameter number. The other is when it is a parameter with X,Y,Z .... axis with their own separate values.
Caution !! remember that you must change the parameter number back at some point within the program and if the program is stopped within the middle of this change there remains the possibility to cause severe damage ( Crash your machine )
Thanks guys this is what I was looking for. I'll give it a shot and see if it works.
Thanks
MudNation
Be careful if/when you change your parameters because the values are machine specific.
Mactec54
Your statement was “A G10 has nothing to do with Rapids or Feed Rate, it is only used for Coordinate system”.
As you can see after your recent post, that statement was clearly incorrect.
This was already covered in what I posted, in the PDFQuote:
Originally Posted by Hardym1
If you had of posted more information than you did, we would not be having these wasted posts, using a G10 is mostly used for X,Y,Z coordinate movesQuote:
Originally Posted by Hardym1
The use of G10 by itself can not do a feed rate change, the codes/letters you use with it is what makes it possible to change feed rates
So clearly what you posted in Post ( 4 ) is incorrect as I said
The Fanuc PDF I supplied clearly states how it can be used with Fanuc controls
So lets get this clear, a G10 can not change Rapids or feed rates by itself, it's the code/letters used with it that does the Rapid/Feed Rate changes, which you failed to have in your post ( 4 )
Hmm, G50.6 Pxx.xx will programatically alter the feedrate override on the lathe here at work. G50.6 p33.33 for example will set 100% rapid to 33.33%. I had been curious for awhile if there were any other machines with similar codes. The machine is a Nanotech 350FG. The control is based on a FANUC control, I am not sure which version. Also, mactec54 is correct with respect to G10. You can use it to change just about any parameter on the machine depending on which letter code you use along with it.