Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: C.Michael on December 09, 2006, 01:07:25 AM
-
I drew a little part in auto cad and then sent it to Lcam..Set it all up..Looked good when it displayed..Then sent it to Mach 3..It looks good in the display..Mach will be cutting just fine and then all of a sudden it goes wildly off course..you can see the proper blue lines before and then the yellow cut course in the display just goes wildly off course,and it goes crazy with the speeds too!! The router itself goes with this crazy line forgetting about limits for speed too...What is going on here?? Michael
-
Can you post you code for us to look at?
-
I think I did it right..Let me see
-
It will cut all the drill points real easy and make all the circles..It goes over to the outside profile and start cutting fine...then it goes off..taking the mill with it...as the off course line is being drawn yellow on the screen,my mill screams trying to keep up..I don't know...when you line jog the code line by line it follows okay..Michael
-
I ran the thing again off line...same thing...
-
Michael,
I don't know. I'm no Gcode guru like some of the others. Are those leadin, out moves? If they are rapids, ( G0 ) they will ignore the feed rates and run at max. Can you post your DWG. file? Different color lines represent something. I don't know what the green means.
-
The outside profile is a closed polyline...the circles are just circles..The outside rectangle is set up to cut up high,so it actually doesn't cut anything on the machine..I just made it that way because that was the piece of scrap wood I had to make this piece..
-
Here is the code I get for the outside profile.
-
i think if you used lazycam to generate the code you didn't use autoclean
-
Here is my version including the holes,
Updated 09/12/2006
Graham.
-
Is your IJ mode set to absolute? It ran fine on my PC ( simulation mode) with IJ set to incremental. Also, only your first G42 has a D1. Every G42 needs a D1, and you also need the tool diameter for tool1 set in the tool table.
-
His program has a G91.1 in it, also D1 is global as far as I know.
Graham.
-
Ok here is something else to add to the mix..When I run it without a tool being selected...TOOL 0...it runs just fine ,no problem except there is no offset..When I put in TOOL 1...that is when it goes off...Graham ,this is what was throwing me for a loop on that wing rib that you helped me on..It finally worked properly with the tool offset when I put in a P.0625 at each and every G41 down the list..Putting in the TOOL1 is what is messing this up
ger21...I checked the IJ mode..yes it is set to absolute ...I have the tool diameter set at .125
Graham..what is the G91.1 and how is it getting in there,if it not suppose to be there?
-
I don't get it, it works fine here.
Tool 1 offset are set to :-
dia = .125
length =0
wear dia = 0
wear len =0
Here is the mach path and the code I used to do it.
-
Michael,
What version are you using?
Graham,
What version does it do good on for you?
-
I am running R1.84.00...When I simulate the run,that is the only thing I am changing..The Tool 1 ..or...Tool 0..I created a new modified code by inserting the P.0625 at each G41..I am going to try that now..Will let you know..Graham..when you ran my original tap file,did you put in a TOOL ..?or was it set to TOOL 0 ..? also when you rewrote the code, you took out the drill points..which is fine,because I don"t think that has anything to do with it..And on my original tap,the drill points and the holes ran fine until it got out on to the outside profile..which is weird because it will start just fine on the profile, maybe a third of the way and then off it goes..and when it goes off,it is where there is a straight line and then it hits a curved line..Right where the two lines meet..But the profile was drawn in Autocad using a closed polyline,so there is no gap there..Michael
-
Well..It didn't work with the G41 all having P.0625...Tool 0...It did the crazy course again...Here is the screen shot and the modified tap file with all G41 P.0625 ...in it..If you are able to make my file run on your machine,then I must have some bug in mine..What gets me is I have two computers running this with the same results..Computer one is the one inside that I design on and one outside in the shop where the mill is...same results...I must have some bug or something...
-
His program has a G91.1 in it, also D1 is global as far as I know.
Graham.
Graham, the D1 didn't appear to be gloabal for me. Only the first circle was comped.
Michael, I think there are some comp (G41/G42) bugs in 1.84. Try it with the latest version.
-
Graham, I just checked and the D1 is not modal for me. Try this. Use .25 for the diameter of tool 1.
-
Apologies Gerry, you appear to be right, that is a major problem and needs to be corrected.
The repercussions of it are huge. For one it meens that any form of subroutine using external D command are out.
I think this needs pointing out to Art and Brian.
Graham.
-
I guess that I will try the newer version..Do I need to uninstall the 1.84 version before installing the new version??
-
Yes, uninstall the older. Before you do, back up your XML. file, screen set, and if you have any KeyGrabber profiles, back those up as well.
-
The XML file is in the Mach folder?? is this where my settings for things like pin settings and motor tuning are??..I live pretty plain..no screen sets or key grabbers ...after backing up the XML file , do I just insert it into the new Mach folder with my licence too?
-
You shouldn't have to unless there is a problem. You're only backing them up as a precaution, in case they are overwritten.
-
I could not sleep thinking about this, so i am back.
I ran the file on 2.007 but when I have gone through the code I have put a D on every G41/42 line so thats why it looks fine as far as the offset been on.
Graham.
-
Well,I took off the older version and installed version R2.0.024...It worked!!! Graham..sorry about your sleepless night,but I can tell that you are a dedicated Man to this subject and you take this moderator stuff seriously!!..But I just can't believe that I am the only one that has had this going off course problem..Anyway maybe this will be the end of it...This G41-42 stuff..Putting in a P (radius) works for me if that is what needs to be done..Or a D # if it works that way too..Thank you Gentleman for the hard work..Michael
-
:)
-
Hi Guys:
Sorry, I only just caught this thread. You dont need anything after a G41, the currrent tool will be used, You can use the P to sepcify a diamter, or a D to specify a tool to get the diamter from.
Radius comp has had alot of work done to it lately, it was buggy on some file before. Take note there are two modes, the original mode is selected in the config/ports&Pins/mill options, or you can select advanced comp. Advanced comp is easier to use, it does have as many rules to using it, but it was buggy for soem file types, depended alot on the moves. Always simulate a comp program offline first to be sure it isnt opne with trouble. Send me any tap files that are a problem, its how I fix the comp, I keep tweaking it to recognise that code..
Thanks
Art
-
I second Graham's :)
EDIT
Make that Super Tropper Graham!
Hey, anybody see that movie?
-
Hi Guys:
Sorry, I only just caught this thread. You dont need anything after a G41, the currrent tool will be used,
But make sure you have an M6 T# to set the current tool. By default the current tool in my setup was tool #0.