LinkBack URL
About LinkBacks
Hi all;
I am new member. I have some problems, and need your help. Please tell me how to post the issues to the forum.
| | |
Hello,
I've been planning on using mastercam to create g-code programs for a KM-3. I was wondering if anyone has any samples of code so that I can know how it is structured. I need to know if it uses work offsets (G54, G55, etc), canned cycles, etc. Does the code need to have a percent sign at the beginning and end?
Thanks
Hi all;
I am new member. I have some problems, and need your help. Please tell me how to post the issues to the forum.
here is a simple drilling program generated from mastercam x3 for the hurco vmx42. I am assuming it should be similar in nc to the km-3.Originally Posted by MadPickinSkills
%
(PROGRAM NAME - 3877F1 )
(DATE=DD-MM-YY - 01-09-10 TIME=HH:MM - 14:48 )
N10 G0 G17 G40 G80 G90
( 1/4 CENTERDRILL TOOL - 4 DIA. OFF. - 0 LEN. - 4 DIA. - .25 )
N11 T4 M6
N12 G43 H4
N13 G0 G90 G54 X.25 Y-.25 S1200 M3
N14 Z.1 M8
N15 G99 G81 Z-.05 R.1 F1.5
N16 G80
N17 M5
N18 M9
N19 G91 G28 Z0.
N20 M01
( 1/4 DRILL TOOL - 5 DIA. OFF. - 0 LEN. - 5 DIA. - .25 )
N21 T5 M6
N22 G43 H5
N23 G0 G90 G54 X.25 Y-.25 S600 M3
N24 Z.1 M8
N25 G99 G83 Z-1.1 R.1 Q.1 F3.2
N26 G80
N27 M5
N28 M9
N29 G91 G28 Z0.
N30 M01
N31 T4 M6
N32 G91 G28 Z0.
N33 G90
N34 G0 Y9.
N35 M2
E
Thanks Shane
Shane's code won't work on your ultimax since it's ISNC formatted for the winmax control.
There are no G5x work offsets. Canned cycles for drilling/boring/tapping only.
Here are some examples of the older Hurco HNC format, be aware that these are all metric programs. G71 = Metric, G70 = Inches. When you select the units in Aux>Change Editor, your selection only effects the graphics. You can switch units in your program just like any other control.
Simple bolt circle. G61/G64 are for turning on/off precision cornering mode, which can smooth out the plunges and retracts on a peck drill cycle. You can probably get rid of them for a quill Z axis.
G83 Z[incremental depth, always positive] Z[first peck] Z[additional pecks]
%
G71G75G90
G0X0.Y0.T11M6
S821M3
X250.0Y150.0
Z3.0M8
G61
G83Z28.0Z13.0Z5.0F159
X200.0Y236.603
X100.0
X50.0Y150.0
X100.0Y63.397
X200.0
G80
G64
G0Z25.0
M25
X0.Y0.M5
M2
E
Roughing out a round pocket:
%
G71G75G90
G0X0.Y0.T3D3M6
S4000M3
X169.25Y120.0
Z3.0M8
G1Z0.03F1700
Y145.0Z-1.976
Y120.0Z-3.982
Y145.0Z-5.988
Y120.0Z-7.994
Y145.0Z-10.0
G3X169.25Y145.0I155.0J145.0
G3X163.629Y170.646I107.938J145.0
G3X139.001Y179.743I146.766J162.88
G3X169.022Y180.587I155.0J145.0
G3X116.263Y177.838I145.66J121.295
G3X94.681Y129.616I135.872J140.122
G3X107.014Y184.654I155.0J145.0
G2X82.404Y160.814I-12.553J283.462
G3X70.292Y128.762I102.447J134.926
G3X70.292Y128.762I155.0J145.0
G0Z25.0
M25
X0.Y0.M5
M2
E
Should be enough to get you going.
gthlm's samples are correct.
File starts with a single "%" and has an "E" as an End of File tag.
If running DNC mode tell your CAD/CAM to remove spaces as it just wastes bandwidth.
Note: Arc I J values are ABSOLUTE not Incremental.
Fixed cycles are a bit different as well. Note that some cycles use multiple Z addresses. Also drill depth is the unsigned incremental value from the Z position the fixed cycle was called (the retract plane).
Confused yet...
N# are purely optional - I put N# only at tool change or optional stop / restart points.
Thanks. Now if I could just get it to connect to a pc.
When I took MasterCam 8 in school years ago, I was able to get
a post processor from MC for my KM3.
I will see if I can find the disc I put it on (floppy)
I never used it as I had communication problems to the PC
Check with MC, and just say Ultimax II Post
So is there no tool length/height offsets? (G43)
The Z height offset is loaded when you do the "Txx M6".
Posting Permissions
| | |
