CNC G-code wants

On-Topic
Lets start to put in small subroutines or methods into this section. Get real code and if there is a trick to use, show the trick.
Martin H. Eastburn
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

There's no tricks to programming. But there is tricks to setups. Here's one... Lets say you hava a big semi flat area to machine. Because of corner radii or angular floors you are forced to use a ball mill. Tilt the thing on a sine plate, say 5 or 10 degrees. Now you will be cutting on the ball as opposed to the tip, quadrupling cutter life and greatly increasing surface finish. Bore a hole somewhere to draw on your cam proggy for pickup.
Programming tricks...hmmmm maybe x and z shifts on a lathe? Maybe doing math like picking up an arc with 3 points? Or using cutter load in programming, or adding music to the end of programs using beeps or blinking lights? be specific?
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Ok Vinny here goes
Let say we are going to make a plate flat on top then drill 4 holes, then countersink each of them.
[ a practical version or altered version of a 4 hole domino. ]
What is the brute force way ? What is the smart to be expanded upon way ? What is the smart way to do it with nominal issue to expand?
Not everyone is a master of all CNC programing code or G-code as some say.
I'm just starting - I do CAD and CAM and CAD-CAM most any day and have done it for a while with 10 and 15 mil endmills.
Martin
Martin H. Eastburn wrote:

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Martin H. Eastburn wrote:

Martin K.
    Probably manual programming at the control.

    Probably programming in a CAM system.
    Here's the code Gibbs spits out for a Fadal. From startup screen to posting the code took 9 min. 36 sec. That's drawing the geometry, choosing tools, selecting the processes. I must be slipping (I did have a couple of false starts), I didn't think it would take over 5 mins.
    That's face milling the surface with a 3" inserted face mill. Spotting the holes with a .375 90 degree spot drill, to leave a .275 chamfer diameter. Drilling the holes .250 dia X .600 deep. Assuming the plate to be .500 thick after facing.
===========================================================% N1O1*PLATE.NCF N2* FORMAT: CNCVIS1 [M8] M756.15.1.PST N3* 2/23/09 AT 8:26 PM N4* OUTPUT IN ABSOLUTE INCHES N5* PARTS PROGRAMMED: 1 N6* FIRST TOOL NOT IN SPINDLE N7T1M6 N8* OPERATION 1: ROUGHING N9* WORKGROUP001 N10* TOOL 1: 3. FACE ENDMILL N11S10000M3 N12G17G90G0X3.472Y1.8333E1 N13Z1.H1M8 N14Z.1 N15G1Z0.F200. N16G8 N17X-1.5 N18Y.6667 N19X1.5 N20Y-.5 N21X-3.5 N22G0Z1. N23G0G90M5M9 N24G53Z0 N25M1 N26T2M6 N27* OPERATION 2: HOLES N28* WORKGROUP001 N29* TOOL 2: .375 SPOT DRILL N30S7500M3 N31G17G90G0X0.Y1.E1 N32Z1.H2M8 N33M46 N34Z.1 N35G81G99X0.Y1.Z.0875R0.1F40. N36X1.Y0. N37X0.Y-1. N38X-1.Y0. N39M47 N40G0G80Z1. N41G0G90M5M9 N42G53Z0 N43M1 N44T3M6 N45* OPERATION 3: HOLES N46* WORKGROUP001 N47* TOOL 3: .25 DRILL N48S7500M3 N49G17G90G0X0.Y1.E1 N50Z1.H3M8 N51M46 N52Z.1 N53G83G99X0.Y1.Z-.6518R0.1Q.25F40. N54X1.Y0. N55X0.Y-1. N56X-1.Y0. N57M47 N58G0G80Z1. N59G0G90M5M9 N60G53Z0 N61X0Y0Z0E0H0 N62M30 % ===========================================================
--
BottleBob
http://home.earthlink.net/~bottlbob
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
BottleBob wrote:

    Oops. Forgot the minus sign on my spot drill. Should have been -.462 on the depth. I would have caught that if I had rendered it, but shortcuts, ya know. LOL
--
BottleBob
http://home.earthlink.net/~bottlbob
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
I had that happen to me few times. Did not want to waist time rendering (specially if it took few minutes) and it cost me dearly. I have a bad habit of finishing pockets bottoms by cheating with the depth value. Say pocket is roughed out 0.99" deep I finish by telling Gibbs to start at 0.9" and finish at 1.00" in 2 cuts. The problem is if there is a rad on my tool. Than Gibbs compensates to whatever dia at 0.005" or 0.01" from cutters end. I try now to make it a point to render even simplest of programs. Jerry

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Jerry wrote:

Jerry:
    Yeah, I ALWAYS render when making parts, it catches a lot of simple boo-boos. But for a newsgroup posting that no-one would ever use I just left it out, both times. Double Oops.     I drew and programmed the whole thing over from scratch in 5 min. 41 sec. put the holes in a different location AND rendered it. Corrected code is below.     I will say the exercise was informative in that it showed me how quickly you can lose your edge in just 4 months of non-use of a CAM system. But it comes back pretty quick.
==================================================% N1O1*PLATE 2.NCF N2* FORMAT: CNCVIS1 [M8] M756.15.1.PST N3* 2/23/09 AT 10:56 PM N4* OUTPUT IN ABSOLUTE INCHES N5* PARTS PROGRAMMED: 1 N6* FIRST TOOL NOT IN SPINDLE N7L0100 N8* SUB NUMBER: 1 N9Y-.7071 N10X-.7071 N11Y.7071 N12M17 N13M30 N14T1M6 N15* OPERATION 1: ROUGHING N16* WORKGROUP001 N17* TOOL 1: 3. FACE ENDMILL N18S10000M3 N19G17G90G0X3.472Y1.8333E1 N20Z1.H1M8 N21Z.1 N22G1Z0.F200. N23G8 N24X-1.5 N25Y.6667 N26X1.5 N27Y-.5 N28X-3.5 N29G0Z1. N30G0G90M5M9 N31G53Z0 N32M1 N33T2M6 N34* OPERATION 2: HOLES N35* WORKGROUP001 N36* TOOL 2: .375 SPOT DRILL N37S7500M3 N38G17G90G0X.7071Y.7071E1 N39Z1.H2M8 N40M46 N41Z.1 N42G81G99X.7071Y.7071Z-.1375R0.1F40. N43L0101 N44M47 N45G0G80Z1. N46G0G90M5M9 N47G53Z0 N48M1 N49T3M6 N50* OPERATION 3: HOLES N51* WORKGROUP001 N52* TOOL 3: .25 DRILL N53S7500M3 N54G17G90G0X.7071Y.7071E1 N55Z1.H3M8 N56M46 N57Z.1 N58G83G99X.7071Y.7071Z-.6518R0.1Q.25F40. N59L0101 N60M47 N61G0G80Z1. N62G0G90M5M9 N63G53Z0 N64X0Y0Z0E0H0 N65M30 % ==================================================
--
BottleBob
http://home.earthlink.net/~bottlbob
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Thanks!
I have code to verify my code and another. So somewhere I learn more and more.
Wish I had a mill in the shop. Someday I will. Just have to make more room and more big bucks!
Martin
BottleBob wrote:

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Martin H. Eastburn wrote:

Face mill, drill, c'sink.

Facemill, integrated drill-c'sink.

Semifinish facemill, integrated, drill-c'sink, finish facemill. The trick here is you now have a perfectly flat face that's not affected by any mushrooming that might occur with tool wear.
I bring this up since I am assuming there are 10 other shops within 3 miles that can do it just as fast and just as cheap. It's never about the code or the control.
-- Bill
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.