Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: viz on January 15, 2013, 03:07:42 PM
-
Hello,
I am trying to solve the problem, but don't understand what is wrong with mach3.
I am using Rhino 5 full version, and MadCam 5 full version. Yesterday i wrote .nc code and everything was working fine it was cutting by path, green dots showing how it will cut.
Today i tried the same code and getting errors, green dots are not cutting by blue path, you can see it at attached picture.
I am using the correct post processor for MadCam, it is Match3_metric. The same problem i have with Edgecam, also the same problem was with RhinoCam. Correctly working only SheetCam. The radius of corners are R4 and R3.1. Endflat mill is D6.
Mach3 is set to MM. IJ mode is set to Absolute.
Mach3 version is R3.043.066
Attaching also .nc code.
-
It may be better if you post a drawing of what the slot should look like as the code is creating arcs from line segments for some reason, you should only have about 15 lines of g-code to produce 2 slots with rads in the corners.
Graham
-
bad export, sorry, will attach new file
-
Attaching .dxf. I was writing pocketing from 3d model by selecting pocket's curves, in simulation it shows that everything is fine. Can't attach .stp file as 3d model.
-
Also made .nc file in sheetcam from this attached .dxf file. As you see it works fine in mach3 from 2d lines. But then i try to use 3d models from other software like Edgecam, MadCam, RhinoCam, i have the same problems above.
-
Sorry for spamming but i want to describe this situation as much as possible. If i import to Edgecam 2d .dxf file and write .nc code, mach3 works good, but if i make the same with 3d model, i get the same problems, that green dots are not going exactly by blue path. I don't know is it mach3 problems or cam software, but i don't think that all 3 different software can make the same bad results.
-
IF your 2.5d Cam programs can create proper code then I think you have a problem in the 3d side of your CAM.
Mach3 can ONLY follow directions based on the Gcode program.
Just a thought(;-) TP
-
Try this code and see what you get :-
%
O0001 (2 SLOTS)
G21 G40 G80 G17
N1 (FLAT 6MM)
G54 G00 G90 G49 X14.733 Y14.674
S18000 M3
Z21.
G01 Z15. F300.
X13. Y15.9 F3000.
G02 X13.1 Y16. R0.1
G01 X56.9
G02 X57. Y15.9 R0.1
G01 Y14.1
G02 X56.9 Y14. R0.1
G01 X13.1
G02 X13. Y14.1 R0.1
G01 Y15.9
X14.733 Y14.674
G00 Z21.
X15.444 Y33.687
G01 Z15. F300.
X13. Y35. F3000.
G02 X14. Y36. R1.
G01 X106.
G02 X107. Y35. R1.
G01 Y33.
G02 X106. Y32. R1.
G01 X14.
G02 X13. Y33. R1.
G01 Y35.
X15.444 Y33.776
G00 Z21.
M30
%
Graham
-
Yes it working perfect, because all corners are orange color. And green dots are going exactly by blue line.
Also it is working for me if i write .nc codes with SheetCam, or write .nc code in Edgecam from 2D lines.
But it is not working if i write .nc code from 3d models creating the same pocketing or roughing option. All corners are blue color from 3d models.
I don't understand what is the problem.
-
When you are creating the rads from the 3d model you are extracting a set of line segments not an arc.
You need to create and arc from the lines or extract an arc, I don't use Edgecam so I don't know how to tell you how to do it so you will have to ask there Tech guys or get on there forum for help.
Graham
-
So the same will be with MadCam ? And all other cam software ?
-
I guess so as they all work in a similar way, you have to turn 3d data into a 2d line to put a tool around it, If you extract an arc as line segments it causes all sorts of problems with tool comp and the like so its worth finding out how to do the job right, its not Mach that is at fault here.
Graham
-
Thank you for your help ! I will try to learn how to write .nc files for 3d models.
-
I don't understand anything, today i downloaded .nc file witch i attached in first post and now it is working perfect !?!? I didn't changed anything, didn't installed or uninstalled any programs and didn't change any settings. Now the green dot go by blue path exactly.
Yesterday windows was updating 3 updates before shutdown. Can it be a reason ?
-
Ok here we go again:
First i have writed to MadCam support, because i was thinking it's madcam postprocesor problems, but they looked and told me it's mach3 problems.
When i am cutting, somehow cnc machine cut one corner is with radius, another one is ok. But it should be both not rounded !
Attached pictures.
-
Attaching .nc file and toolpath pictures, "back ploted" is from madcam support, they told me that everything is ok. I need to check problems in controler.
Also attaching .dxf file.
As you can see all coners are not rounded, but somehow machine cut one corner with radius another one without
-
Attach your xml file you are using.
Try this....reverse the cutting / path direction ( in your cam ) and see if it reverses the radius to the other side of that cut
when run in Mach.
I don't use any of the software that you are using so no help on them.
RICH
-
looking at the code you have no G02 or G03 commands so the issue has to be related to the CV settings you have set, increase the look ahead and reduce the feed by half for a start and then see what the difference is.
Graham
-
Thank you, i will try to reduce the feed rate. But it's not very big, 3000mm/min.