Problem- Lathe JohnFord with Fanuc 18 - need help

[longgo]

Hi to all,

The point of that post is asking for advice.I know that here is the place where is possible smart people, skkilled in CNC programing , to give me idea am I in deep mistake if I wish to continue to work that proffesion.
My experience is mainly with centers with 5 axes,and for a last I touch lathe 12-13 years ago..
The machine is JohnFord ST 240B with CNC - FANUC 18iTB.It is possible to use rotary tools for miling and driling also.It has 2 normal axex "X,Z" , and with command M91 it goes from spindle mode to axis mode , and M90 turn it back. Axis "Y" give the abilities to make pokets and other things and max movement is +/- 83mm.And here is my pre entered question:

QUESTION: did I'm right to think that this machine have some crush, because on indication(position) , when it goes in reference point , shows "0" to all axes(for C is 359.99) , but on "Y" shows 0.6mm My colegue told me everytime in all offsets to put dat value "Y -0.6" because in other case it will not work properly.Well.. when I just ask why not put that "small" mistake in that parameter which is responsible for zero point and that will dismist that everytime inserting, the answer was : it's not necessary,just remember to put it(like - i told you that this is rule!)





The machine produce axes made from usual normal iron(soft iron) with sizes D100-:-130mm and lenght from 800 to 5800mm.It has 5 hidraulic steady-rests which has 40mm in with ball-bearings on which the part suppouse to rotate.
And now let me to start:

I'm sorry for that bad and ugly drawing, but for that prupose it will do the result( i hope )





(the size D125 with tolerance 0/-0.1 are for ball-bearing)
The way of clamping is to use one center with bolts:



the other part is again center, on long tail..





I'm sorry abot the quality of that pictures , but they are made only with phone.

QUESTION 1: Is it possible to use that jaw free, and is it produce any vibration:





if I use it directly. The point of that question is that for longest ones they used that roller with eight bolts:




The main idea of that is to prevent that normal disbalance and jumping.Suppose to be used as the first all bolts are untwisted,after that the hidraulic jaw take it and with 2 indicator clocks and manage that bolts we made that "jumping" around 0.01mm.
I'm thnik that is not a problem to use that steady rest jaw directly, but the only problem is that trace of sliding wich will be apeared.

(maybe i'm wrong..)

QUESTION 2: on that scheme You'll see the way of mesuring of RENYSHOW. The machine has one anglular pipe with something square on top for tool mesuring


This "H" means in which side to mesiure the tool in example: going to MDI mode, (the tool is near , about 1-2mm near to position 8), and write:
G65 P9011 H8 T2(for tool 2).

That will put mesured value for X offset in position 2




Now the other fast problematic question - when i ask why there is written only R value for miling tools but nothing for that lathe-knife-inserts (in example R0.8..or R1.2 and so on..) the answer was that it working only for miling.That is, who it is...!!That is FANUC 18.., and even in 6-th series there was that possibility to write the R of the inserts , and to program the contur only for teoretical edge and machine automatik add R and so on..!?!?
I ahven't experience with that CNC type and that is the point that I wish to know.. is it true?

QUESTION 3: Here first I'll show how that guy make all thing and after that mine ideas.. and will be so thanksfull for that if You told me did i'm in such a big misstake,even to try to think...




First he clamp position(on that picture) 1, after that 2,3.. absolutely without 4,and then the chuk.
The zeroes of coordinate systems are: G54 on that visible site,the other G55 to other korner(that surface which is catched with bolts for the center)
His program:


:108

G54 G99(G99 directly cutting speed)
G50 S1200(turns limit)
M44 (gear use - faster , up to 2000 tpm)
??....(Raw right tool with R1.2)
G96 S220 M3(G96-feed per turn)
G0 Z3.

X130.
G1 X121.5 F0.4
Z-197. M8
G2 X127.5 Z-199.8 R3.0
G1 X129.
X126.Z-200.

Z-683.
G0 X400. M9
Z3.
M01
G54 G99
G50 S1200

M44
??....(right finishing - R0.8)
G96 S240 M03
G0 X123. Z2.
G01 X117.6 F0.4
G1 Z120.06 Z-1.4 F0.1 M8

Z-197.5 F0.18
G02 X125.06 Z-200.4 R2.5
G1 X130. F0.5
X124.8
Z-282.F0.22
X124.95

Z-519 F0.14
X124.8 F0.1
Z-682.F0.22
G0 X400. M09
M01
G55 G99

G50 S1200
M44
T..(raw left with R1.2)
G96 S220 M3
G0 X450. Z-2.
X130.

G1 X121. F0.35
X126. Z103.8
Z345.
G00 X450. Z1000. M9
M5
M01

G55 G99
G50 S1200
M44
T...(left finishing with R0.4)
G96 S240 M3
G0 X450. Z-2.

X117.6
G01 Z0 F0.2 M8
X119.7 Z1.4 F0.1
Z-2. F0.5
X119.66
G1 X124.95 Z103.79 F0.12

Z345.6 F0.22
G00 X450. Z1000. M9
M5
M00(cleaning the steady-rest-on the picture in the middle)
G54 G99
G50 S1500

T.... (end mill with inserts D25,3 - blade,R0.8 insert radius)
G97 S2200 M4
M91(spindle goes to rotary axis mode)
M54(clam the jaw)
??8
(from here he goes to that dialog mode and fill form for poketing)

G1900 D120. L250. K0
G1050 L10. J4. K2. H2. F0.2 V0.2 E0. W1. B2. C2. Z2.
M98P8053(that is subprogram with strange kodes..for moving on that work..)
G0 X360. M9
M90
M55(open jaw)

Z20. M5
M00
G54 G99
G50 S1500
T..(end mill , D20, 2 blades, insert R1.4)
??91

G97 S2400 M4
M54
M8
G1050 L10. J7. K0. H0. F0.2 V0.2 E0.5 W1. B2. C2. Z2.
M98 P8053
M90

M55
G00 X360. Z200. M9
M5
M30.


I can't understand two things.. why in example i to make wrong if i write like that:


G54 G99 G50 S1200 M44
??....(tool)

All the time was raw pointed that the machine accept only that way:

G54 G99

G50 S1200
M44
??....

I'm sorry but in that manual which goes with the machine,and my experience with FANUC told me that the only problem is if I use two M kodes on the same line and that is not every time..

Also when I ask what is the way to drill a hole or somthing like that .. and wish to use cycle G83 .. I can use only that format:
G00 X112. Z...(goes to position)

G83 X90. F...(make a hole)
G0 X130.
(goes away..)
--- When i ask - why You not remove the G83 function he wrote that:
G00 X112. Z...
G83 X90. F...
G80

G0 X130.
He told me to not think that is center, that is lathe and all is so diferent...

For me that is somthing not so acceptable.In the manual was that:


which explain me that i CAN!! write that piece of code::

G00 X120. Z...

G83 G98 X90. R2. Q2. F.. M27(when use the spindel like axis,that put spindle break on)
G80 G0 X130. M28(break off)

and guess what was his answer - No, it's not working that way..!?!?
Now I ask someone who had experience with that machine or/and CNC - Is it true?



Now let me to show my way and program:
I suggest if I use that way of tool mesure(which is exactly like on that scheme):




it mean that i'll work with the theoretical nose of the tool- is it? Even if I deceide to use G41/42 function?
And so.. I try to put the values in that R position into the offset, which was stoped right away from my colegue!


And the program created by me:
:108
#2002=0.8(??02-Right)
#2004=0.8(??04-Left)
(Because usually we put a little extra up to X wering offset, make first finishing and after that calculate what we need , and make it final, for that reason we put all the time 0.8mm more,because i'm sometimes forgot this and that,put that variable and in every start of program it load that values into the offset)
N1 G54 G0 X400. Z10. G99 G50 S1000 M44(???°x. moving in X axis in plus is 483????)

T1212(R1.2 - raw/right hand)
G96 S220 M3 G71 P10 Q35 U1. W0.5 F0.22
N10 G0 X121. Z-2.
N15 G1 X118. M8
N20 X120.05 Z-0.7
N25 Z-197.5

N30 X125.05 Z-200. R2.5
N35 G0 X400. Z3. M9
N40 M01(..)
G54 G0 X400. Z2. G99 G50 S1000 M44
T0202(R0.8 - finishing/right hand)
G96 S240 M3 G70 P10 Q35 F0.1

N45 M01(..)
G55 G0 X400. Z-3. G99 G50 S1000 M44
T0303(R1.2 - raw/lefthand)
G96 S220 M3
-- here is the place that i calculate the cone and i do it in this way:




G0 X120.8 Z-2.
G1 Z0 F0.22 M8
X125.8 Z103.
Z746.
G0 X400. Z-3. M9

N50 M01(..)
G55 G0 G99 G50 S1000 M44
T0404(Finishing lefthand - R0.8)
G96 S240 M3
X118.36 Z-2.
G1 Z0. F0.12
X119.84 Z0.7

X124.95 Z103.
Z346.
(here i deceide that if the tool is not moving so much on X axis when make that two bearing places is much espetially in case that the tolerance is 0.0125mm between their 2 axes, will be good idea - do the both atonce)
Z507. F0.8
Z745. F0.12
X124.8

Z827.4 F0.2
U-0.2 W0.4 F0.1
G0 U4.
Z345.
G1 X124.8 F0.06
Z508. F0.2

G0 X400. M9
G54 Z30. M5
N55 M00 (before milings , check and clean)
M91(switch to from spindle to normal axis)
??54(close jaw)
G54 G0 G99 X380. Z20.

T0606(end mill 3 inserts,D25.Here I cant understand how is possible to make R1.5 exactly R1.5 if previos tool is R0.8!??! When i suppose to make that in ceter machine all the time I use 1-st R2. for raw, and then R1.4 for next clean R.He simply told me - it's not a problem, please dont think about it..)
G96 S250 M4
X[120.05-11] Z[#2906+2](here I put the tool corner/end 2mm near to the surface,and just take that R from the offset via that variable for 6-th tool)
#1=[120.05-11]+14(14mm up is that other kontur where start that R on Z200mm)
WHILE [#1 GE [120.05-11]] DO1
G19(choose YZ plane)

G41 Y15.9 Z0 F0.6
Z-200.
G3 Y-15.9 R15.9
G1 Z2.
G40 Y0 Z[#2906+2]
G18

#1=#1-2
END 1(that movement will be with spen in via 2????, and will be made 7 times)
G0 X380. Z20. M9
N55 M01
G54 G0 G99 X380. Z20.
T0909(endmill 2 inserts,D20-R1.5)


G96 S250 M4
X[120.05-11.1] Z[#2909+2]
G19
G41 Y15.97 Z0 F0.4
Z-200.
G3 Y-15.97 R15.97

G1 Z2.
G40 Y0 Z[#2909+2]
G18
G0 X380. Z20. M9
M55(open jaw)
M90(turn back to spindle mode)

M30
%

That was my program, but he told me that even if it work on simulator that is dificult and hard and will not work in real mode.The other thing is that the inserts we use for finishing (small picture) produce that king of chips ....



and this from the other site make the surface bad.. and with bumps..The explanation from his site was - Dont try to think if exist that good for that work, kind of insert i'll take it..(and i've seen before that kind.. whit spots and so on ant when they work, they make the chips on smal part.. like raw tool)

I'll be so greatfull to everyone who will chek that and told me .. did i'm so wrong to think that can work trhat stuf..If You think that is funny that cost me one good job because my colegue told to the boss that i cant learn fastt enaugh,.. and .. they released me..
Thaks alot!

[adekunle]

pls.kindly send me the user manual for fanuc vmc 750 and the simulator.

[longgo]

Originally Posted by adekunle pls.kindly send me the user manual for fanuc vmc 750 and the simulator.

sorry, i have not that.. Hope someone else will have it and share with You, or try via torrent systems. Sometimes it is possible to find there.


Regards

[PixMan]

Wow, that's a LONG post here.

Your first paragraph & photo: Note that the "Machine" coordinate values are all at zero. After sending the axis home, execute a "G50 Y0". This will make the Absolute and Relative values read zero also. There should be no need for having any "crush" zone set. That is something set in the parameters 1320-1326 range, the "soft limits".

Question 1: Yes, you should be able to run without that steady rest on the workpiece, but you will have to have a well-balanced part and a free-cutting insert. I would definitely have the steady rest engaged for the milling operation though.

Question 2: The turning tools should also have a value for the "R" register, matching the tool nose radius of the insert IF you also use a G41 or G42 tool compensation code in your part program. If you do use the "R" value together with G41/G42, you will have to also have a value in the "T" register for tool nose orientation. The most commonly-used T codes are 2 or 4. Check you manual for relating to your machine. The tool setter will not set that, you have to input it manually. The tool setter SHOULD set the T code correctly when you touch off on the "h5" or "h7" sides of the setter. You should NOT have to execute any G65 code, the toolsetter should put the machine & control into it's toolsetting mode when you swing it into position.

Question 3: I don't have time to read and compare both your programs, but I can say that you are trying to do more than is necessary with setting the tool R and T values with variables coding. Use the tool set mode of the machine to set as much as possible, add only the R value that the setter cannot detect.

If I read the last part of your posting correctly, you've been terminated from working on this anyhow. If not, get a completely different insert for finishing. That one appears to be a semi-finish/roughing insert, and with a shallow depth of cut you get the bad "rat's nest" of chips. A good finishing insert will control that.

[longgo]

Originally Posted by PixMan Wow, that's a LONG post here. Your first paragraph & photo: Note that the "Machine" coordinate values are all at zero. After sending the axis home, execute a "G50 Y0". This will make the Absolute and Relative values read zero also. There should be no need for having any "crush" zone set. That is something set in the parameters 1320-1326 range, the "soft limits". Question 1: Yes, you should be able to run without that steady rest on the workpiece, but you will have to have a well-balanced part and a free-cutting insert. I would definitely have the steady rest engaged for the milling operation though. Question 2: The turning tools should also have a value for the "R" register, matching the tool nose radius of the insert IF you also use a G41 or G42 tool compensation code in your part program. If you do use the "R" value together with G41/G42, you will have to also have a value in the "T" register for tool nose orientation. The most commonly-used T codes are 2 or 4. Check you manual for relating to your machine. The tool setter will not set that, you have to input it manually. The tool setter SHOULD set the T code correctly when you touch off on the "h5" or "h7" sides of the setter. You should NOT have to execute any G65 code, the toolsetter should put the machine & control into it's toolsetting mode when you swing it into position. Question 3: I don't have time to read and compare both your programs, but I can say that you are trying to do more than is necessary with setting the tool R and T values with variables coding. Use the tool set mode of the machine to set as much as possible, add only the R value that the setter cannot detect. If I read the last part of your posting correctly, you've been terminated from working on this anyhow. If not, get a completely different insert for finishing. That one appears to be a semi-finish/roughing insert, and with a shallow depth of cut you get the bad "rat's nest" of chips. A good finishing insert will control that.

Anyway .. I'm out of that company exactly because of that .. smart ass that was "helping" me all the time..
Anyway.. i was with idea that is possible that zero mistake to be corrected at ones into the setting parameters and.. to disappear at all but no one espetially He, trust me that this is more easy that all the time to check is it there. About that using of R and so on.. is more easier if You calculate something the system to add that value.. - he explain me that in example 0.8mm the radius of insert i need to calculate also by myself.. - why the f*** i cant use something which is into the cnc from the beginning of 80's?
And about the "nest" ... I was saying exactly the same about inserts..but it was told to me - because u're mill worker You did not understand what is here .. and i just close my mouth. That's the story..
All that mail was produced to see did I'm so wrong or what.. and by the way.. with milling i also thing that is good idea to be fixed at least into the middle of part .. but.. what can we do..

Thanks for answer..