Results 1 to 11 of 11
05-27-2010, 09:27 AM #1
Okuma canned drill cycle G74....What is proper format?
G74 X Z K D L E F
What do the letters designate?
A .500 drill 2" deep. How would it look?
G0 X0. Z.1
G74 X0. Z-2.0 K? D? L? E? F.007
05-27-2010, 10:01 AM #2
Here are some notes that might help ....
(1) X and Z are same as your Fanuc control
(2) I and K are shift amounts ... for example for K ... rapid the tool to Z1.000, call your cycle with a K.900 ... the actual staring point to drill would be Z.100 ... maybe if you had a hole already say 1.00" deep, and wanted this cycle to start at say .900 deep into the part, not at the actual front.
(3) D = depth of cut ( like a peck amount )
(4) L = if you input a value here, each time the tool reaches this value, it goes back out to the start point. For example : doc = .250 L=.500 ... every two depth of cuts the tool will rapid out to the start point.
(5) F = feedrate
(6) E = dwell time at the bottom
Hope this helps .... this is only the drilling side, this cycle is also for grooving ... much more powerful than your Fanuc ever was.
CNC XChange could have told you all this as well as the info in the other posts for Okuma programming and auto-converted your Fanuc program to Okuma format in less than 5 seconds ... leaving more time for actual chipmaking ... ... I'm just saying ...
Check out CNC XChange at Kentech Inc. - Real World Machine Shop Software
05-27-2010, 10:04 AM #3
I got this a while ago from one of the Okuma techs in Denver. It is from a 5000 control, which he said many of the add ons to the 3000 control were like the 5000 control...
I got it trying to figure out how to use the deep drilling cycle that my LC10 supposedly has installed, but it doesnt work for me, so maybe someone will have an idea there... but anyway, here is what I have from them.
Well - scratch that... the TINY file size limits for this forum wont allow a 23.3kb file...
Ill email it to you.
05-27-2010, 10:08 AM #4
According to the Okuma manual for the OSP 700L control, K is shift amoumt in Z axis direction,D is depth of cut(infeed amount), L is total ifeed amount for tool withdrawal motion, and E is duration of dwell when target Z is reached. If I am translating correctly, K is the distance in Z from the initial position to the start of drilling feed,D is the peck depth, L is how far you want to advance between pecks, and E is dwell at the bottom of the hole.
That L is a little confusing. I THINK (?) it means for instance, if you retract 1" and only want to advance .95, then go back to a feed instead of rapid, this is where you accomplish this. Don't bet the farm on it, cause I could be wrong. Since we don't use the L, I'm just giving you my bet guess. We run cast iron almost exclusively, and never peck. Very seldom have to drill in the lathe.
As I said, this is what the book says. If you can interpret that, consistently, then your doing better than me.
05-27-2010, 01:21 PM #5
Russ, I feel for you on this...just when you think you got Jinglish figured out for Fanuc stuff, then you have to learn the Okuma-Jinglish dialect. I have had the same issues with the Yasnac on the Matsuura....
05-27-2010, 03:32 PM #6
When I knew I HAD to go out and get another machine, I kept telling myself....."IT HAS TO BE FANUC, IT HAS TO BE FANUC!"
But once I saw ole ugly Betty run, and checked out her spec. sheet.....I figured....Okuma, Schuma........I can learn that, no problem.
Then when it was sitting on my floor and I couldn't get it to do anything, I kept saying......"WHY THE FU@& DIDN'T I GET A FANUC!!"
But....it's all good now......learning as I go along, and making progress every day..........but deep down inside......still wishing I had got a Fanuc.......
Change is difficult!......at least for me, but it won't be long before I'll be singing praise to my Okuma.....I just know it!
05-28-2010, 03:55 PM #7
So....I want to drill a hole 2" deep for example........
.500" drill 2" deep.
Is this how it should look?
GO X0. Z.1
G74 X0. Z-2.0 D.5 L.1 F.007 E.5
Is that how the code should look?
05-28-2010, 04:56 PM #8
My okuma is sort of touchy about things in the code immediately preceding a code.
Looking at the document I have from Okuma for a 5000 control, the only thing that strikes me as "maybe" an issue is setting the Z starting point in the same line as the first X0
I would go with this, but may not be necessary to have the extra line.
G74 X0. Z-2.0 D.5 L.1 F.007 E.5
After I just re-read the program, I see your L is .1 - not sure your intention there....
Taking that into consideration, your code tells me you would be doing this....
Starting point X0 Z.1
It would want to drill in .5, but is programmed to do a full retract at .1 - so it might not peck at all, and just drill .1 and do full retracts after each...
Do that cycle if it doesnt error out til -2. dwell for .5 second
If you changed your L to 1. instead, I would expect it to drill -.5" and peck to break chips, drill to -1. then do a full retract. Then rapid in to -1, drill to -1.5, peck, drill to -2. dwell .5 sec - adding the G0Z.1 would bring it out to starting point so you could then take it to tool change pos. Other wise, I think it will stop at the bottom of the hole, until you command it out of it.
05-28-2010, 05:26 PM #9
I see what you're saying Wade. I thought the "L" was the retract plane like "R" would be in Fanuc.
You mean it rapids right to the last place it stopped? Yikes....Fanuc stops .1 away and picks up the feed again.
Gotta be some pucker factor in there if Okuma does that.
Thanks for the help!
05-28-2010, 05:43 PM #10
I cant say what it would do for sure, but I would guess, being a drilling cycle, it would stop short and feed in... but I have no idea if Id be right or not.
Im sure youll try it cutting air the first time anyway, so youll know... On the 3000 control, they seem to be fond of .25mm as defaults, so I would guess that maybe it will rapid to .25mm short and feed in... and the peck would be the same...
I bet it will stop short and feed in, but cant promise.
05-29-2010, 10:06 AM #11
Ok Russ, lets look at this one and break it down...this drills a starter hole and then opens up for a finish boring bar.
G95 G97 S150 M3
G00 X0 Z0.2 M08
G74 X1.24 Z-0.75 I0.314 D0.125 L0.375 F0.002 E0.04
This drilling cycle starts at X 0 and drills to a final depth of Z-0.75 and will feed at F0.002 and will dwell at the bottom of the hole for E0.04.
It will Peck at D0.125 increments but will only fully retract every L0.375. That is sort of like a combination of peck drilling and deep hole drilling. If you leave off the L you will stay in the hole until it reaches full depth. The L lets you choose how deep you want to go until the tool retracts fully. To the best of my knowledge the pecking retract distance is set in machine parameters.
The I0.314 is the X distance the tool will offset at the end of each cycle. It will do this until it reaches X1.24. If you didnt have the I value you will get only one hole.
In this application I am using an endmill to first drill a flat-bottomed hole and then open it up using the endmill like a boring bar. This saves me an extra tool in the turret. To see the tool check out the following link and you will see some photos of it and the results.
The Real Help Machine Tool Giveaway
Look at the May 17th posting for the tool photos.
Your code would be better like this,
GO X0. Z.1
G74 X0. Z-2.0 D.5 L1. F.007 E.5
Now your tool will feed at F.007 and peck at each D.5 and will retract fully at L1. until you reach your depth of Z-2.0 and dwell E.5
Let me know if this helps.