CIRCLE MILLING USING VARIABLES
ฝัง
- เผยแพร่เมื่อ 26 ส.ค. 2024
- Learn how to use variables to circlemill a bore without having to write new g-code when changing tool diameter or bore diameter.
O0001 (CIRCLE MILLING USING VARIABLES)
#100=2. (#100 IS DIA OF CIRCLE)
#101=.5 (#101 IS DIA OF TOOL)
(TOOL # AND H# SHOULD BE THE SAME)
(CHANGE RPM AS NEEDED)
(CHANGE FEED RATE AS NEEDED)
N100
G0G90G17G40G80G49G20
G91G28Z0.
T1M6 (T# SHOULD MATCH H# BELOW)
S1000M3 (RPM MAY NEED CHANGING)
G90G0G54X0.Y0.
G43H1Z2.M8 (THE H# SHOULD MATCH TOOL # ABOVE)
G0Z.1
G1Z-.1F20.
G1X0.Y [#100/2-#101] F10. (CHANGE FEED HERE)
G3X0.Y[#100/2-#101/2]I0.J[#101/4]
G3X0.Y-[#100/2-#101/2]I0.J-[#100/2-#101/2]
G3X0.Y[#100/2-#101/2]I0.J[#100/2-#101/2]
G3X0.Y[#100/2-#101]I0.J-[#101/4]
G1X0.Y0.
G0Z2.
G91G28Z0.M5
G28Y0.M9
G90
M30
%
![[UNCUT] The Loyal Pin ปิ่นภักดิ์ EP.4 (4/4)](http://i.ytimg.com/vi/d3l5rxl5CVo/mqdefault.jpg)
Tom, you have the best tutorials I have ever seen by far. I work an entire machine shop by myself with 2 haas CNC machines and 15 years since I've run one. Your training has helped me through some hard parts and keeps USN planes flying. Thank you!
-James
James Shaw Thank you James. That is great feedback!! Let me know if I can answer any questions. Tom
I don't know if I've ever let you know, Tom. But I owe you a huge thanks for having these videos available. I learned the basics, and later macros from your videos.
Thanks!
Andrew Probst
Great tutorial Tom. Saved me a lot of head scratching.
Great video Tom, grettings from Argentina. I'm working on a Doosan 3100xly right now and i'm practicing with variables using milling and turning at the same time...
Tom, you have the best tutorials
thanks
Thanks Leo. I appreciate that feedback.
www.udemy.com/course/cnc-makro-programlama/?couponCode=TEKNIKOKULCNC
You are the master, Sir! Thank you very much!
Should the first g1 movement be [#100/2-#101/4]? I tried using a 3/8 cutter to cut a 1/2" hole, and it wanted to go to a negative that was beyond the size of the hole.
Hey Timothy. A 3/8 tool doesn't give you a whole lot of wiggle room. You may need to consider a smaller tool.
great video Tom!
Great tutorial Tom -Jeff Carpenter
neoblood3d Thanks Jeff.
Hey Tom, your videos are great!......I was wondering if you could help me create s face mill macro program using a 1.6 dialed face mill and just have it have two variables. #1 being length and #2 being width. I am having problems because as I increase the width I need a step over amount to add( maybe .8, half the cutter). Can you help me...Thanks
Sorry you mean , It is useful for different size holes at same time in the same program. Thanks
HI Tom, you are make a good tutorial
thanks
nb : can you make tutorial about tools exchange position please?
( like Robodrill the position for changing tools from the pocket on the right side of carrrousel )
if you start and end at the same place in a circle you dont need an X or Y, just the I or a J.
G3X0.Y-[#100/2-#101/2]I0.J-[#100/2-#101/2]
G3X0.Y[#100/2-#101/2]I0.J[#100/2-#101/2]
could be rewritten in one line of code as:
G3J-[#100/2-#101/2];
makes a complete circle.
Hello bro
Thanks Tom
Can this be done using cutter comp instead of variables? Someone mentioned cutter comp cannot be used when circle cutting. Is this true?
Cutter comp can be used to mill a circle as long as a linear move is used on the line where cutter comp is engaged.
The variables give you much more control of the size of the circle and the diameter of the tool. Hope that helps.
Thanks for watching. Tom
Sir please make one video how to use maltple wcs use hmc machine like 30 deg 90 deg 270 deg 180 deg 0 deg 45 deg 25 deg
Great video, have a question for you. I am kinda new to using macro variables, but was wondering if there is a way when circle milling to add a variable for a step over. Say I wanted to start at one bore size and finish at a different size without having to change the hole size variable each time. Thanks for your help.
You need to set a variable for start diameter and finished diameter, then step distance. Use WHILE DO and work in the math. It can be done.
Hello tom I have a question Can I use logic gates for example OR, AND
#101/4 I couldn't understand this part, why 1/4 and not 1/2?
Is this for machining two separate diameters?
It's the lead-in radius. The .500 dia tool is .250 away from diameter of circle. The radius of .250 is .125, OR .500 / 4=.125. The variable at #101 is the tool diameter, so no matter what tool diameter you put there, the equation is #101 / 4. IE, whatever size tool you use, it will swing the proper radius into the circle diameter that you are cutting.
Hi
may i know how to do the program with depth of cut and width of cut?
tq
Great stuff Sir. Tell me where to ship the whiskey crate that i owe You:)
Excellent tutorial. How we can add multiple passes.(depth)
create a sub for the circle path, then input a z offet.
Hello Tom
Thank you show much . But would you know if this technique will work a DX 32 control for an older Brigdeport ?
www.udemy.com/course/cnc-makro-programlama/?couponCode=TEKNIKOKULCNC
can you show how to draw a pocket on a cylinder pls.
I experimented a little bit with this in Gwizard and i got to the conclusion that i cannot change the coordinates for y, only for x. For y i was not able to do it, so if i want to do multiple holes i have to change my origin every time for the new coordinates. I was wondering if this can be fixed, maybe i missed something. Thank you in advance.
Did you make the cutting portion a subprogram and use a G91 at the beginning?
Plz sir tell me about thread milling in macro program
repeat a cicle???
i have a question?
when using G12 -13,whats the meaning of I and k..i dont think is the same meaning as G02/3
No they do not have the same meaning. The I in a G12 circle milling cycle is the start diameter and the K is the finish diameter. Thanks. Tom.
dont forget the Q for stepover.
We want to learn micro pragram
sorry we can use G41, G42 instead. Thanks
Where is inpur depth of cut?
Mm program mai