[300sniper]

i am new to cnc and am still teaching myself so i have a lot to learn. i have a project i need to do that i am not sure if it can be programmed manually or if it is going to need a cad/cam program for it.

i need to make a 5.725" diameter pocket .375" deep with a .375" radius. it would be easy to do with a 3/4" ball mill but i don't have one. i really don't want to get one for this quick project and not need it again. i was thinking about cutting the flat bottom of the pocket with a 1/2" endmill and using a 1/2" ball mill to cut the radius. i have no idea how to go about programing the radius part of it though.

can this be programmed manually or am i better off just buying a 3/4" ball mill? i don't have any 3d cad/cam programs nor would i know how to use them either.

i'd appreciate any help.

thanks.

[holbieone]

you could trig it out ,but that would take a few

i would be faster with a .75 ball

with a .5 ball you would have scallops

[holbieone]

if you can wait until Sunday i can write a program for you

is your os Microsoft windows

[300sniper]

if you can wait until Sunday i can write a program for you

is your os Microsoft windows

if it's not that big of a deal for you i'd really appreciate it. i would like to keep it as smooth as possible so if .002" step over works for you, that would be great. i am in no big hurry to get it done and have a few weeks so don't go out of you way.

and yes, windows it is.

thanks a lot,
robert.

[holbieone]

it's no big deal ,i have some software I've been writing that i would like to test

I'll need an example of how your machine does circle interpolation

like G2x1.y1.i0.j0.f10.

and can it be run absolute

or i can program it point to point

how big is your program buffer

[300sniper]

it's no big deal ,i have some software I've been writing that i would like to test

I'll need an example of how your machine does circle interpolation

like G2x1.y1.i0.j0.f10.

and can it be run absolute

or i can program it point to point

how big is your program buffer

the circle interpolation you show will work with my machine. it can be run absolute or incremental (i assume that is what you are asking). again i am new to this so i am not sure about the program buffer. is that the length of the program it will take? if so, i have run some programs that were a couple thousand lines long. it is mach3 that came with a tormach.

let me know if you need any more information.

thanks again.

[holbieone]

the circle interpolation you show will work with my machine. it can be run absolute or incremental (i assume that is what you are asking). again i am new to this so i am not sure about the program buffer. is that the length of the program it will take? if so, i have run some programs that were a couple thousand lines long. it is mach3 that came with a tormach.

let me know if you need any more information.

thanks again.

ok then program size should not be a problem

[Andre' B]

Playing around on break I came up with this, not sure if it will run in Mach but it does in NCPlot.

Down feeds and radial outfeeds are set very small, not sure what your machine can handle.

Also you would need to add tool changes and length compensation code for however you normally do them.

(X ZERO CENTER OF HOLE)
(Y ZERO CENTER OF HOLE)
(Z ZERO FINISHED TOP OF PART)
(TOOL CENTERLINE PROGRAMMING)
(THE LINES WITH COMMENTS ABOUT ,FEED PER,)
(CAN BE CHANGED FOR MORE OR LESS CUT PER PASS)
(DURING THE SPIRAL DOWN AND OUT)

(THE LINE WITH THE COMMENT ,STEP ANGLE, CAN)
(BE CHANGED FOR MORE OR LESS CUT PER PASS)
(AROUND THE RADIUS)




(*************)
(PROGRAM FOR)
(1/2 IN FLAT END MILL)
G0X0.230Y0.000
G0Z1.000
G1Z0.100F30.0
()
#1=0.03
#2=0.005(DOWN FEED PER G3)
()
WHILE[#1GT-0.375]DO1
G3X0.230I-0.230Z[#1]F5.0
#1=[#1-#2]
END1
G3X0.230I-0.230Z[-0.375]F5.0
(MAKE BOTTOM FLAT)
G3X0.230I-0.230F5.0

(5.725/2 = 2.8625)
(2.8625-0.375 = 2.4875)
(2.4875-0.250 = 2.2375)
()
#1=0.230
#2=0.005(OUT FEED PER G3)
()
WHILE[#1 LT 2.2375]DO1
G1X[#1]F2.0
G3X[#1]I[-#1]F5.0
#1=[#1+#2]
END1
G1X2.2375F2.0
G3X2.2375I-2.2375F5.0




(*************)
(PROGRAM FOR)
(1/2 IN BALL END MILL)
()
G0X2.4875Y0.000
G0Z1.000
G1Z0.100F30.0
()
#1=0.03
#2=0.005(DOWN FEED PER G3)
()
WHILE[#1GT-0.375]DO1
G3X2.4875I-2.4875Z[#1]F5.0
#1=[#1-#2]
END1
G3X2.4875I-2.4875Z[-0.375]F5.0
(MAKE BOTTOM FLAT)
G3X2.4875I-2.4875F5.0

#1=0.0
#2=0.0
#3=0.0
#4=2.0(STEP ANGLE AROUND 0.375 RAD)
()
WHILE[#3 LT 100]DO1
#1=[0.125-[0.125*COS[#3]]]
#2=0.125*SIN[#3]
G1Z[-0.375+#1]F5.0
G1X[2.4875+#2]F2.0
G3X[2.4875+#2]I[-[2.4875+#2]]F5.0
#3=[#3+#4]
END1

[Kiwi]

Andre'B
Is this all the part that handles the .375 radius?
Am I missing something? I don't see how this handles the changing radius of the cutter.
Just trying to understand.

(1/2 IN BALL END MILL)
WHILE[#1GT-0.375]DO1
G3X2.4875I-2.4875Z[#1]F5.0
#1=[#1-#2]
END1

[Kiwi]

This code is for a 1/2in dia. Ball Nose cutter for the corner only

G01 X2.6125 Y0 Z-0.25
G03 X2.6125 Y0 I-2.6125 J0
G01 X2.6118 Y0 Z-0.2631
G03 X2.6118 Y0 I-2.6118 J0
G01 X2.6098 Y0 Z-0.276
G03 X2.6098 Y0 I-2.6098 J0
G01 X2.6064 Y0 Z-0.2886
G03 X2.6064 Y0 I-2.6064 J0
G01 X2.6017 Y0 Z-0.3008
G03 X2.6017 Y0 I-2.6017 J0
G01 X2.5958 Y0 Z-0.3125
G03 X2.5958 Y0 I-2.5958 J0
G01 X2.5886 Y0 Z-0.3235
G03 X2.5886 Y0 I-2.5886 J0
G01 X2.5804 Y0 Z-0.3336
G03 X2.5804 Y0 I-2.5804 J0
G01 X2.5711 Y0 Z-0.3429
G03 X2.5711 Y0 I-2.5711 J0
G01 X2.561 Y0 Z-0.3511
G03 X2.561 Y0 I-2.561 J0
G01 X2.55 Y0 Z-0.3583
G03 X2.55 Y0 I-2.55 J0
G01 X2.5383 Y0 Z-0.3642
G03 X2.5383 Y0 I-2.5383 J0
G01 X2.5261 Y0 Z-0.3689
G03 X2.5261 Y0 I-2.5261 J0
G01 X2.5135 Y0 Z-0.3723
G03 X2.5135 Y0 I-2.5135 J0
G01 X2.5006 Y0 Z-0.3743
G03 X2.5006 Y0 I-2.5006 J0
G01 X2.4875 Y0 Z-0.375
G03 X2.4875 Y0 I-2.4875 J0

[300sniper]

Playing around on break I came up with this, not sure if it will run in Mach but it does in NCPlot.

Down feeds and radial outfeeds are set very small, not sure what your machine can handle.

Also you would need to add tool changes and length compensation code for however you normally do them.

i am still new to cnc and honestly, i don't understand that. i do appreciate it though.

[300sniper]

This code is for a 1/2in dia. Ball Nose cutter for the corner only

G01 X2.6125 Y0 Z-0.25
G03 X2.6125 Y0 I-2.6125 J0
G01 X2.6118 Y0 Z-0.2631
G03 X2.6118 Y0 I-2.6118 J0
G01 X2.6098 Y0 Z-0.276
G03 X2.6098 Y0 I-2.6098 J0
G01 X2.6064 Y0 Z-0.2886
G03 X2.6064 Y0 I-2.6064 J0
G01 X2.6017 Y0 Z-0.3008
G03 X2.6017 Y0 I-2.6017 J0
G01 X2.5958 Y0 Z-0.3125
G03 X2.5958 Y0 I-2.5958 J0
G01 X2.5886 Y0 Z-0.3235
G03 X2.5886 Y0 I-2.5886 J0
G01 X2.5804 Y0 Z-0.3336
G03 X2.5804 Y0 I-2.5804 J0
G01 X2.5711 Y0 Z-0.3429
G03 X2.5711 Y0 I-2.5711 J0
G01 X2.561 Y0 Z-0.3511
G03 X2.561 Y0 I-2.561 J0
G01 X2.55 Y0 Z-0.3583
G03 X2.55 Y0 I-2.55 J0
G01 X2.5383 Y0 Z-0.3642
G03 X2.5383 Y0 I-2.5383 J0
G01 X2.5261 Y0 Z-0.3689
G03 X2.5261 Y0 I-2.5261 J0
G01 X2.5135 Y0 Z-0.3723
G03 X2.5135 Y0 I-2.5135 J0
G01 X2.5006 Y0 Z-0.3743
G03 X2.5006 Y0 I-2.5006 J0
G01 X2.4875 Y0 Z-0.375
G03 X2.4875 Y0 I-2.4875 J0

that definatly looks right. what kind of a finish do you think that will leave? i would like to make it as smooth as possible. did you come up with that by hand or a program? how difficult would it be to set the z increments to .002"?

i really appreciate it.

[jcoats]

There is a program called simplecnc that is pretty cheap. If writes g-code snippets for pickets, circles, etc. It would give you some hints on howto write g-code.

[turmite]

Not knowing all your set up I made this one for you using Rhino and Madcam. The program starts centered .5" above the surface of your pocket. Standard Madcam Mach3 inch post processor. I encourage you to raise your z axis a couple of in. and run this in the air! Otherwize......(nuts)

I did not set feed rate though it may be in the post, but I failed to look.

Mike

[holbieone]

Not knowing all your set up I made this one for you using Rhino and Madcam. The program starts centered .5" above the surface of your pocket. Standard Madcam Mach3 inch post processor. I encourage you to raise your z axis a couple of in. and run this in the air! Otherwize......(nuts)

I did not set feed rate though it may be in the post, but I failed to look.

Mike

use caution if you run this tape "snipr.tap"

he has the serface .5 below "Z" 0

he uses one tool ,thats ok if you know what corner radius was programmed for the tool

the tape has "0" spindle rpm and 100 ipm feed rate

the tape has a lot of strange moves in it "i would plot it out first"

and the fillet you want doesn't look correct ,but that's hard to tell not knowing what corner radius he used for the tool

looks like he's coming out of the radius and breaking the corner

[300sniper]

use caution if you run this tape "snipr.tap"

he has the serface .5 below "Z" 0

he uses one tool ,thats ok if you know what corner radius was programmed for the tool

the tape has "0" spindle rpm and 100 ipm feed rate

the tape has a lot of strange moves in it "i would plot it out first"

and the fillet you want doesn't look correct ,but that's hard to tell not knowing what corner radius he used for the tool

looks like he's coming out of the radius and breaking the corner

i just downloaded ncplot and see what you are saying. something is not right with it. the code that kiwi posted looks real good but i think i am going to want a tighter step over/down.

i do appreciate the help guys.

[Kiwi]

that definatly looks right. what kind of a finish do you think that will leave? i would like to make it as smooth as possible. did you come up with that by hand or a program? how difficult would it be to set the z increments to .002"?

i really appreciate it.

The code is for 16 turns which gives a step along the arc of 0.037in and a cusp of 0.0002in.
The larger the cutter, the truer the arc. As a 1/2in (0.25in radius) is close to your 0.375 corner, not that many passes is required to give a reasonable finish.
I have a program which I wrote to generate the code.
Z steps of 0.002 equals 187 passes which is way over kill.

The attached program is a continuous helix for the corner which wont leave a mark at the step down.

[300sniper]

The code is for 16 turns which gives a step along the arc of 0.037in and a cusp of 0.0002in.
The larger the cutter, the truer the arc. As a 1/2in (0.25in radius) is close to your 0.375 corner, not that many passes is required to give a reasonable finish.
I have a program which I wrote to generate the code.
Z steps of 0.002 equals 187 passes which is way over kill.

The attached program is a continuous helix for the corner which wont leave a mark at the step down.

thanks a lot. i really appreciate your help. i am new to this and i have a lot to learn, especially when it comes to 3d.

when i get this going, i'll post up how it went.

[turmite]

use caution if you run this tape "snipr.tap"

he has the serface .5 below "Z" 0

he uses one tool ,thats ok if you know what corner radius was programmed for the tool

the tape has "0" spindle rpm and 100 ipm feed rate

the tape has a lot of strange moves in it "i would plot it out first"

and the fillet you want doesn't look correct ,but that's hard to tell not knowing what corner radius he used for the tool

looks like he's coming out of the radius and breaking the corner

You are absolutely correct. I failed seperate the two tool paths. One should have been with a 1/2" endmill doing a pocket to the bottom of the part and out to the start of the .375" radius.

I don't mind you commenting on my post, but at least use it all. You failed to mention, I told him I had not looked at the code, nor had I checked the post processor, and I told him to use it with caution, I also included where the starting point of the program would be. Just in case you missed it.........I included it for you!

"""Not knowing all your set up I made this one for you using Rhino and Madcam. The program starts centered .5" above the surface of your pocket. Standard Madcam Mach3 inch post processor. I encourage you to raise your z axis a couple of in. and run this in the air! Otherwize......

I did not set feed rate though it may be in the post, but I failed to look."""

Mike

[turmite]

holbieone thanks for the catch. I went back to redo the code and check everything and I found I had used the 5 axis module which I know has a couple of post bugs in it. The feedrate is in the post processor, though I don't used this, because I am a wood worker and 100ipm is slow for the most part. I will get that corrected. I also saw the odd moves, and honestly I am not sure what caused that. I recoded it using another strategy and it came out perfectly.

With that said, I don't want to post till sniper tells us what materials, feedrate etc. If he is actually going to use the code, it needs to be right.

My original zip had two bits, a 1/2" flat end mill and a 1/2" ball. I failed to apply a number to the bits and the program wrote the code as one bit rather than two.

Sniper tell us what you want/need, and someone will deliver!

Mike

ps this just goes to prove another long know fact! Never do this kind of work when you are not at yourself. Too tired and lots of pain are not the time to be trying to do something like this.