Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Armenias on August 19, 2011, 12:10:47 PM
-
Good morning everyone, and thanks for any help you will be able to bring to me..
I meet a problem using Mach3 mill, when I load some gcode files using arcs, Mach3 gives me the error written in the title.
I read some similars topics, and tried to change IJ mode to "Inc" instead of "Absolute", but everytime I import my DXF file, the IJ mode switch automatically in "Absolute"..
Can you help me ?
Thanks a lot.
William
-
CHange the settings in your CAM program to ONLY use incremental IJK OR make sure it includes the Gcode call to switch the Function at the machine from Inc to Abs.
Inc IJK is the normal approach.
Hope that helps, (;-) TP
-
Okay, that sounds good, I use SolidWorks to make my DXF's files. I'll try to find any solution on it ..
Thank you
-
(;-) THE dxf file is NOT the cut file (Gcode) you have to change the way the CAM program interprets the dxf when it converts it to Gcode. Set it to ONLY use INC IJK.
Hope that helps, (;-) TP
-
I do not undersdand,
I make my DXF file on solidworks, import it to Mach3 and I generate Gcode with Mach3 ..
So I set mach3 to INC, but it does'nt work !
I am sorry if I am missing something ..
-
MACH3 itself cannot generate gcode from a DXF file. UNLESS you are talking about a very early Mach2 version where it could import and convert a dxf.
The normal path to gcode is
CAD(dxf) ---> CAM(Gcode) ------> Mach3
The cad is where you create the drawing and export it as a DXF, such as "NewPart.dxf"
The cam is where it takes the DXF and converts it into a Gcode FIle such as "NewPart.tap" ( THiS is where you need to set the CAM to only use INC IJK when it creates the Gcode file)
Mach3 takes the Gcode and runs the Gcode and makes the newpart.
(;-) TP
-
Okay thank you very much ...
I still don't understand why Mach3 allows users to import DXF files...
Let's find a good cam ..
Thank you again !
-
Are you refering perhaps to LAZY CAM that comes with mach3????
(;-)TP
-
Exactly ... thank you.. I thoughr I understood all with loading directly DXF files... I think I have to restart since the beginning, using lazycam makes wrong or unfinished pieces..
Thank you
-
(;-) Lcam uses the standard INC ijk convention for arcs. I am not sure how they are getting mixed up in your Gcode files.
Could be another program changes the Setting via Gcode and then when you go back to a regular file it is backwards.
(;-) TP
-
using lazycam makes wrong or unfinished pieces
It does what it is told to do. Same goes for any other program. Read the manual.
Same goes for any other CAM program. No program can read the users mind on how they intend on doing something.
Let me clarify........my bride of many years may be able figure me out. ;)
RICH
-
Let me clarify........my bride of many years may be able figure me out. ;)
RICH
But I am betting you cant figure her out even after all these years ;D
Hood
-
Got that right Hood,
Gave up after she told me that "it took her so many years to get me just like she wanted me and now she's not sure who I am" ???
Ya just got to love em........... :-* Men are from Mars and Females are from Venus :P
Easy to get confused at times ;) That's why a shot and a beer can put things back into perspective.
Burp ;D
RICH
-
;D
-
Never used it but from a quick look it appears that LazyCAM posts either inc IJ OR abs IJ depending on how you set it on the Post Gcode option screen. Either way it EXPLICITLY posts a G90.1 or a G91.1 in the code preamble. So unless I'm missing something Mach can NOT get the mode wrong regardless of what you might have set previously in Config/General Config. Mach simply switches mode according to what is POSTED. Although a mis-match of IJ mode WILL cause this error I don't see how this can be the case in this instance. The ONLY time the operator has to make sure Mach and CAM modes match is when the CAM DOESN'T explicitly post the mode. There are other reasons why you might get the error in your title and I suspect that's the case here.
Ian
-
Thank you Rich for youre very intelligent response,
I'll read it, but after some research, I think that finally, DXF's files made on Solidworks are quite not compatible with lazycam.
Stirling, thank you for you response. I had this problem only when I was using Import dxf's file's option on Mach3, now with lazycam, there is no radius problem, excepted a wrong or unfinished piece.
Can I post one of my dxf files then you try to open it on lazycam ?
Thank's
Ps : there is a DXF attached, after using lazycam, I get this quite wrong g-code :
N5 (File Name = tata on Saturday, August 20, 2011)
N10 (Default Mill Post)
N15 G90.1
N20 G0 Z1.0000
N25 M3
N30 X35.0000 Y-47.0000
N35 Z0.1000
N40 G1 Z0.0000 F60.00
N45 Y-33.0000
N50 G0 Z1.0000
N55 X32.0000 Y-30.0000
N60 Z0.0000
N65 G1 X-32.0000
N70 G0 Z1.0000
N75 X-35.0000 Y-33.0000
N80 Z0.0000
N85 G1 Y-47.0000
N90 G0 Z1.0000
N95 X-32.0000 Y-50.0000
N100 Z0.0000
N105 G1 X32.0000
N110 G3 X35.0000 Y-47.0000 I32.0000 J-47.0000
N115 G0 Z1.0000
N120 Y-33.0000
N125 Z0.1000
N130 G1 Z0.0000
N135 G3 X32.0000 Y-30.0000 I32.0000 J-33.0000
N140 G0 Z1.0000
N145 X-32.0000
N150 Z0.1000
N155 G1 Z0.0000
N160 G3 X-35.0000 Y-33.0000 I-32.0000 J-33.0000
N165 G0 Z1.0000
N170 Y-47.0000
N175 Z0.1000
N180 G1 Z0.0000
N185 G3 X-32.0000 Y-50.0000 I-32.0000 J-47.0000
N190 G0 Z1.0000
N195 X-66.0000
N200 Z0.1000
N205 G1 Z0.0000
N210 G2 I-70.0000 J-50.0000
N215 G0 Z1.0000
N220 X-66.0000 Y50.0000
N225 Z0.1000
N230 G1 Z0.0000
N235 G2 I-70.0000 J50.0000
N240 G0 Z1.0000
N245 X70.0000 Y60.0000
N250 Z0.1000
-
Hi Armenias
Your DXF works fine in LazyCAM and it produces good code on my system. I'm thinking you're running an unlicenced demo version which is restricted to the number of lines it'll handle. Hence your gcode is not wrong - it's just not complete.
Ian
-
In fact I use a demo version, but I didn't know that demo version was restricting the number of lines. If it's true, I buy it tonight ..
Thank's a lot Ian
-
Every thing works perfectly ! Except a scale problem on mach3 (distance divided per 2), but i'll find the solution..
Thank you everybody !
-
hello all. I know this is an old thread but i am getting this Radius error and changing the IJ setting from absolute to incremental in Mach 3 is not solving it. I have been stuck with this for months and not able to test out my CNC machine. Any help would be GREATLY appreciated. Below is the code i tried, but i am getting it on multiple codes that i have tried. This is just a simple hexagon i created to test the machine.
( Made using CamBam - http://www.cambam.co.uk )
( 9_6_14 shape 9/7/2014 3:41:24 PM )
( T0 : 0.0 )
G20 G90 G91.1 G40
( T0 : 0.0 )
T0 M6
( 9_6_14 shape.nc )
( Made using CamBam - http://www.cambam.co.uk )
( 9_6_14 shape 9/7/2014 3:19:32 PM )
( T0 : 0.0 )
G20 G90 G91.1 G40
( T0 : 0.0 )
T0 M6
( 9_6_14 shape.nc )
( Made using CamBam - http://www.cambam.co.uk )
( 9_6_14 shape 9/7/2014 8:49:11 AM )
( T4 : 0.25 )
G20 G90 G91.1 G40
( T4 : 0.25 )
T4 M6
( 9_6_14 shape.nc )
( Made using CamBam - http://www.cambam.co.uk )
( 9_6_14 shape 9/7/2014 8:49:05 AM )
( T4 : 0.25 )
G20 G90 G91.1 G40
( T4 : 0.25 )
T4 M6
( 9_6_14 shape.nc )
( Made using CamBam - http://www.cambam.co.uk )
( 9_6_14 shape 9/7/2014 8:47:13 AM )
( T0 : 0.0 )
G20 G90 G91.1 G40
( T0 : 0.0 )
T0 M6
( 9_6_14 shape.nc )
( Made using CamBam - http://www.cambam.co.uk )
( 9_6_14 shape 9/7/2014 8:45:25 AM )
( T0 : 0.0 )
G20 G90 G91.1 G40
( T0 : 0.0 )
T0 M6
( 9_6_14 shape.nc )
( Made using CamBam - http://www.cambam.co.uk )
( Untitled 9/6/2014 3:11:34 PM )
( T4 : 0.25 )
G20 G90 G91.1 G64 G40
G0 Z0.125
( T4 : 0.25 )
T4 M6
( Profile1 )
G17
M3 S1000
G0 X-0.5644 Y0.9009
G1 F10.0 Z-0.25
G1 F30.0 X-1.2356 Y0.6539
G3 X-1.3932 Y0.5046 I0.095 J-0.2581
G1 X-2.6154 Y-0.8468
G3 X-2.6222 Y-1.2079 I0.204 J-0.1845
G1 X-1.2159 Y-2.885
G3 X-0.8481 Y-2.9341 I0.2107 J0.1767
G1 X1.6519 Y-1.1945
G3 X1.7646 Y-0.9158 I-0.1571 J0.2257
G1 X1.3376 Y1.2613
G3 X0.9728 Y1.4664 I-0.2699 J-0.0529
G1 X-0.5644 Y0.9009
G1 F10.0 X-0.5298 Y0.807
G1 F30.0 X-1.2011 Y0.5601
G3 X-1.3066 Y0.4513 I0.0604 J-0.1642
G1 X-2.5412 Y-0.9139
G3 X-2.5456 Y-1.1437 I0.1298 J-0.1174
G1 X-1.1393 Y-2.8208
G3 X-0.9053 Y-2.852 I0.1341 J0.1124
G1 X1.5947 Y-1.1124
G3 X1.6665 Y-0.9351 I-0.1 J0.1436
G1 X1.2394 Y1.242
G3 X1.0073 Y1.3726 I-0.1717 J-0.0337
G1 X-0.5298 Y0.807
G1 F10.0 X-0.5126 Y0.7601
G1 F30.0 X-1.1838 Y0.5131
G3 X-1.2619 Y0.4262 I0.0432 J-0.1173
G1 X-2.5042 Y-0.9474
G3 X-2.5072 Y-1.1116 I0.0927 J-0.0838
G1 X-1.101 Y-2.7886
G3 X-0.9338 Y-2.8109 I0.0958 J0.0803
G1 X1.5662 Y-1.0714
G3 X1.6175 Y-0.9447 I-0.0714 J0.1026
G1 X1.1904 Y1.2324
G3 X1.0245 Y1.3256 I-0.1227 J-0.0241
G1 X-0.5126 Y0.7601
G1 F10.0 X-0.5644 Y0.9009
G1 Z-0.5
G1 F30.0 X-1.2356 Y0.6539
G3 X-1.3932 Y0.5046 I0.095 J-0.2581
G1 X-2.6154 Y-0.8468
G3 X-2.6222 Y-1.2079 I0.204 J-0.1845
G1 X-1.2159 Y-2.885
G3 X-0.8481 Y-2.9341 I0.2107 J0.1767
G1 X1.6519 Y-1.1945
G3 X1.7646 Y-0.9158 I-0.1571 J0.2257
G1 X1.3376 Y1.2613
G3 X0.9728 Y1.4664 I-0.2699 J-0.0529
G1 X-0.5644 Y0.9009
G1 F10.0 X-0.5298 Y0.807
G1 F30.0 X-1.2011 Y0.5601
G3 X-1.3066 Y0.4513 I0.0604 J-0.1642
G1 X-2.5412 Y-0.9139
G3 X-2.5456 Y-1.1437 I0.1298 J-0.1174
G1 X-1.1393 Y-2.8208
G3 X-0.9053 Y-2.852 I0.1341 J0.1124
G1 X1.5947 Y-1.1124
G3 X1.6665 Y-0.9351 I-0.1 J0.1436
G1 X1.2394 Y1.242
G3 X1.0073 Y1.3726 I-0.1717 J-0.0337
G1 X-0.5298 Y0.807
G1 F10.0 X-0.5126 Y0.7601
G1 F30.0 X-1.1838 Y0.5131
G3 X-1.2619 Y0.4262 I0.0432 J-0.1173
G1 X-2.5042 Y-0.9474
G3 X-2.5072 Y-1.1116 I0.0927 J-0.0838
G1 X-1.101 Y-2.7886
G3 X-0.9338 Y-2.8109 I0.0958 J0.0803
G1 X1.5662 Y-1.0714
G3 X1.6175 Y-0.9447 I-0.0714 J0.1026
G1 X1.1904 Y1.2324
G3 X1.0245 Y1.3256 I-0.1227 J-0.0241
G1 X-0.5126 Y0.7601
G0 Z0.125
M5
M30
M30
M30
M30
M30
M30
M30
-
Sunburned,
Your file backplots fine and Mach Mill runs it with no errors when I tried it out.
Post your xml file and someone will have a look.
RICH
-
Thanks for the help. My XML is attached. Please let me know if you need anything else. I had to rename it so i could post it.
-
bump
-
Just wanted to check on this. Any help would be great.
thanks
-
No errors reported here using your xml file.
RICH
-
I was hoping something would be found. If anyone has any other ideas I would be happy to try them out. Right now I have a very big and expensive paperweight.
-
Code works fine here. See pic ....
RICH
-
The file you posted in reply #21 is not an XML file. It's a copy of the program MachXML.exe. Please post your xml PROFILE file. That's the one ending in .xml in your Mach3 folder with the same name as the profile you're using.