can anybody write a CNC program for lathe please.?

[Yogesh K. Raman]

quote:

---

The part i want a program is simple

ppl say.can i send the file to you please.

if u can help me i will be nice

---

I don't know much English but that surely sounds like you want harass Colin.

 

Put your CATIA drawing picture on the forum, it will be more accesible to everyone, and not you alone can learn but share them as well to all forum members.

[bala_51083]

"if u can help me it will be nice "

thats wht i meant it was a typo...thts it.

i never knew i typed such a thing to colin till now..

[Storkman]

I am not a lathe man, but there are some very good ones in here. Put your file on the ftp and I am sure one of them will take a look at it and give you some advice.

[Don S at Barefoot CNC South]

bala

Put it up on the ftp and I will take a look, I have both catia translators.

[Jack Neelands™]

Then Bala i owe you an appology if your statement is true and I'll flog myself for penance (maybe ShopWench can help me) for my Antagonizing posts.

 

If not I'll just get ShopWench to flog me anyway

[4xxx4]

I'm a lathe guy - e-mail me your drawing and I'll see what I can do. I will do a quick hand write if possible and I'll give ya a few tips for setting up the simple operation of the machine to keep it safe.

Can ya scan the "G-code" and "M-code" lists from the book and send them as well? It really helps to have the syntax the machine needs.

 

[email protected]

[bala_51083]

 

 

this is the part we want to machine.if any body can help it will be nice.

 

Thanks '

Bala

[crazy^millman]

Then I will also put myself as one to aplogize as well.

 

A simple program for you are could be:

 

G0 Z.1 X-.05(APPORACH MOVE)

G42 G1 Z0( APPORACH PART AND TURN ON RIGHT CUTTER COMP)

G1 X0(MOVE TOOL TO CENTER)

G3 X3.937 Z-1.9685 R1.9685(COUNTER CLOCKWISE ARC MOVE)

G3 X3.7179 Z-3.2635 R1.9685(COUNTER CLOCKWISE ARC MOVE .05 PAST ARC)

G40 X4.0 Z-3.4(MOVE TO POSITION TURNING OFF CUTTER COMP)

G0 X4.2

G0 Z.25

 

 

Now this is not a complete program and will only make the 1st part of the arc there. If I was making this part I would make the stub end 1st roughing the radius. I would then grab that in a set of soft jaws and then do the other side. and finish the radius with either comp code like this or centerline tool code that take the radius of the tool in to account like the example above. It is hand written and done real quick with a calucator.

 

HTH

 

[ 09-27-2006, 09:29 PM: Message edited by: Crazy^Millman ]

[ShiftZ]

Ahh yes, the "simple" accuracy test. If you gents have no experience on CNC machinery may I suggest you get the dude in that shop who does because according to that dwg your little test will require two set ups. BTW, little rads work just as well as big ones and only require one safe op.

[ShiftZ]

This may work and it may not, depends on your control and my math(you take your chances in here man). No garunteees.

 

%

:0001

 

N1

(ROUGH TURN)

(CNMG 3/32 TOOL NOSE RADIUS MINIMUM)

G99

G50S1400

G0T0101

G97S700M3

G54X8.25Z.2G96S500

M8

G71U.1R.02

G71P100Q101U.005W.002F.012

N100G0G42X-.065

G1Z0

X0

G3X7.874W-3.937R3.937

G1Z-5.25

X8.25W-.05

N101G0G40X8.25W.2

G28U0W0M9

M0

 

N2

(FINISH TURN)

(VBMT 3/32 TOOL NOSE RADIUS)

G99

G50S2500

G0T0303

G97S700M3

G54X8.0Z.1G96S500

M8

Z-3.8

G71U.04R.02

G71P200Q201U.005W0F.012

N200G1G42X7.874W0

G1Z-3.987

G3X7.4254W-1.31R3.937

G1X8.0

N201G0G40X8.0

G0G40X8.0

Z.1

G42X-.065S600

G1Z0F.01

X0F.007

G3X7.4254W-5.247R3.937

G1W-.05

X8.25F.03

G0G40X8.5W.2M9

G28U0W0

M0

M30

%

 

[ 09-27-2006, 10:04 PM: Message edited by: ShiftZ ]

[bala_51083]

thank you guys.i will try to understand the program,with a manual for this machine i ordered.

[ShiftZ]

Be carful to stand your blank off of the jaws a little as you may feed/rapid into them. Do the math on that back ark and give yourself about 1/2" of room.

[ShiftZ]

Your control may be of an older type. If it is it won't understand "R" as being a radius value.

In that case I and K are used to indicate arc rotation. It may also not read decimal places in the feed rates.

.007 would look like 70 in that case and .012 would be 120 etc. As stated before I don't promise anything.

 

 

%

:0001

 

N1

(ROUGH TURN)

 

 

(CNMG 3/32 TOOL NOSE RADIUS MINIMUM)

G99

G50S1400

G0T0101

G97S700M3

G54X8.25Z.2G96S500

M8

G71U.1R.02

G71P100Q101U.005W.002F120

N100G0G42X-.065

G1Z0

X0

G3X7.874W-3.937K-3.937

G1Z-5.25

X8.25W-.05

N101G0G40X8.25W.2

G28U0W0M9

M0

 

N2

(FINISH TURN)

(VBMT 3/32 TOOL NOSE RADIUS)

G99

G50S2500

G0T0303

G97S700M3

G54X8.0Z.1G96S500

M8

Z-3.8

G71U.04R.02

G71P200Q201U.005W0F120

N100G1G42X7.874W0

G1Z-3.987

G3X7.4254W-1.31I-3.7127K.05

G1X8.0

N201G0G40X8.0

G0G40X8.0

Z.1

G42X-.065S600

G1Z0F100

X0F.007

G3X7.874W-3.937K-3.937

X7.4254W-1.31I-3.7127

G1W-.05

X8.25F300

G0G40X8.5W.2M9

G28U0W0

M0

M30

%

[bala_51083]

quote:

---

G71P100Q101U.005W.002F120

---

i was trying to understand the program, wht does the P and Q here do...?

[gcode]

P100 = N100 (start of the roughing loop)

Q101 = N1o1 (end of the roughing loop)

 

The lines N100 through N101 define the toolpath roughed by the G71 canned roughing cycle

[4xxx4]

P and Q also define the finish tool path. When they are called by G70 they tell the control to look back for the sequence of this program section and the tool follows just the path described in those blocks. G70 can also be used without a roughing cycle as long as the blocks are numbered and that it describes what you want the tool to do.

Also, do you really want a 200mm dia. part or 100mm ? If you want a 100mm sphere from a lathe then you cut the radius in 1/2..... This is a very large test object but it will cover a larger section of the machine envelope for a more thorough test.

 

I use a "safe start" program to tell the machine to clear the part for tool change position. It takes a lot of clutter from the program and when doing a lot of hand writing it makes it much faster to put all the prep command stuff in it. I can usually have my machine programmed and set up faster than programming it with a CAM system.

 

I did these from memory - I'm in wire EDM now, but you should'nt have much problem getting this going.

 

:0001(SAFE START PROGRAM)

G00 G40 G97 M9

G99

T0X10.Z10. (SAFE INDEX POSITION)

M99

 

 

:0002(PRODUCT 1 RADIUS OP)

(8.0 DIA ALUM IN JAWS)

(JAWS 1.2 DP @ 400 PSI)

N1(RUF TURN CNGP432 .032 RAD)

M98P1(SAFE START PROGRAM)

G50S2000

G0T0101G96S1300M3

X8.0Z.2/M8

G71P11Q12D.1U.01W.002F.011

N11G0X0(G42 OPTIONAL)

G1Z0F.002

G3X7.874Z-3.937R3.937

G3X7.4699Z-5.182R3.937(PROBLEM LINE)

(JUST USE G1 Z-5.182 TO CUT STRAIGHT)

X8.F.02

N12G0Z.2

M98P1

M01

N2(FINISH TURN VNGP331 .016R)

M98P1

G0T0303G96S1300M3

X8.Z.2

G70P11Q12F.002

M98P1

M30

[Namliek_J@TheeCircle™]

quote:

---

Make sure to leave yourself enough time to sweep up the chips before you leave.

---

Hey Colin, make sure you stop by the local bakery and bring in fresh doughnuts for everyone, and be there early enough to have coffee made.

 

[mcpgmr]

quote:

---

I suggest you get the dude in that shop who does because according to that dwg your little test will require two set ups

---

shiftz, This can actualy be done in one setup if your careful and use the correct strategy. I've done lots of parts on the lathe like this. Worst case is you might have a tiny nipple left over from parting off. Just my two cents.

[4xxx4]

MMMMMM, Dognuts....

 

I agree that this could be made in 1 operation but doing the radius as a "back end" type feature would require using tools that are not as accurate as doing the radius in a "front side" operation with conventional turning tooling. The 8" diameter makes it difficult to get a long enough tool behind the part and still maintain rigidity. Also, when this 8" diameter part comes off the remaining material blank, it will need a rather large catchers glove to grab it....... I don't know about you but I wouldn't feel safe trying this. Not to mention that it would still require another operation to remove the "nipple" precisely for the application.

2 set ups would be the way to go for a complete part but if they only need to do the radius end for a CMM to probe it, then just the radius would be sufficient.

 

So Bala, Does it sound real simple any more? There are a lot of things to consider when programming any machine and this is why we are called "Professionals".

[mcpgmr]

quote:

---

MMMMMM, Dognuts....

---

[bala_51083]

i appreciate all your help guys.I know you guys are professionals,thts the reason why i asked you guys for help.

 

Thanks

Bala

[4xxx4]

quote:

---

quote:

--------------------------------------------------------------------------------

MMMMMM, Dognuts....

--------------------------------------------------------------------------------

 

 

---

Yeah, I know. It is kinda wierd that they are the breakfast of champions AND cops.....

[ShiftZ]

Flippin bunch "O" whackos in here I tell ya.

[ShiftZ]

Did someone say nipple?

[ShiftZ]

No wait, it was xxxx!! Ya it was xxxx!! Muwahahahahaha.........xxxx, or was it nipple?