Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: N4NV on February 10, 2009, 04:43:14 PM
-
I used the OD arc 3 wizard to generate the following code. All of the code is not listed just the part leading up to the problem. The G-code roughs the part OK (it looks like a ball on a rod). When it gets to the I and K part in the finish cut, it cuts right through the ball and leaves a smooth cut like it was a straight G1 move. It appears to display properly in the preview window. Any idea what could be wrong (I am still working on learning I's, J's and K's).
G1 Z-0.1196
G0 X0.155 Z-0.1096
G0 X0.195
G0 Z-0.1904
G0 X0.155
G1 X0.135 Z-0.1804
G1 Z-0.198
G0 X0.155 Z-0.188
G0 X0.195
G0 Z-0.09
G0 X0.125
G1 Z-0.1184
G0 X0.145 Z-0.1084
G0 X0.195
G0 Z-0.1916
G0 X0.145
G1 X0.125 Z-0.1816
G1 Z-0.198
G0 X0.145 Z-0.188
G0 X0.195
G0 Z-0.09
(Pass at FinishCut)
G0 X0.12
G1 Z-0.1181
G2 X0.12 Z-0.1819 I-0.0025 K-0.0319
G1 Z-0.198
G0 X0.14 Z-0.19
G0 X0.195
G0 Z-0.09
F1
(Pass for Final Dimension)
G0 X0.116
G1 Z-0.12
G2 X0.116 Z-0.18 I-0.0005 K-0.03
G1 Z-0.2
G1 X0.175
G0 X0.3
I should add that my settings were X start 0.1750 Xend 0.1160 Filler Radius 0.0300 Z start -0.1000 Z end -0.2000 Z center -0.1500 clearance 0.0100 Finish pass cut 0.002.
Thanks
Vince
-
VINCE,
Didn't try your code, but i always look / dry run in MACH Turn . Find the bad line since manny times its just a XZ move and you need to just have one or the other first or as individual moves.
RICH
-
VINCE,
Didn't try your code, but i always look / dry run in MACH Turn . Find the bad line since manny times its just a XZ move and you need to just have one or the other first or as individual moves.
RICH
I guess I a little puzzled in that the code looked good in the preview window. I thought Mach would cut what was shown. I did do a dry run, but the movement is so small, only about .05" total in .002 steps and there are so many moves happening so fast, I could not tell it cut through the final arc.
Vince
-
Vince,
Don't be puzzled because after trying your settings in the wizard and posting the code something is not right.
What is shown in the turn window seems to agree with the code, but, if you dry run it in MACH it is not following the pathing
and you already know it will cut right through it. Just a short break at work so no time to fool around.
What version of Mach are you using?
RICH
MODIFIED: SEE LATER REPLY
-
I have two different lathes, one running version 3.042.008 and the other 3.042.020. Both versions do the same thing.
Vince
-
Have you got Mach set to Inc I&J's or Abs?
Graham
-
Vince,
I have not actualy cut the attached code file based on your posted wizard inputs.
The attached two files show screen prints of dry runs in Mach3 Turn. 1_ is for mach version
3.042.010 and the other is for 3.042.020. They are attached to show that there is no " cut thru the ball"
in Mach Turn simulation.
I forgot that, with a high rapid / feed rate, that the "simulation" in the newer version will not portray the pathing
correctly. Thus the pathing, when run, shows a cut thru the ball. As you know turn will be getting some attention in the near future.
Will actauly cut it this weekend. BTW the only mod i did to the file was changing the initial XZ move to x then z.
RICH
-
Have you got Mach set to Inc I&J's or Abs?
Graham
They are set for incremental. I tried it both ways and got the same results.
Vince
-
As you know turn will be getting some attention in the near future.
RICH
So I was told by Brian in York, PA. There is some really strange things going on in MachTurn besides this little problem. I started going through my Smid book an studying up on turn G-code and found that MachTurn does very little of what is industry standard. I also had a very strange problem on my CHNC. I upgraded from version 3.042.008 to 3.042.020. When I did my M6 tool change macro started working funny. The turret would start indexing before it reached the tool change position and it no longer would see the turret index fault switch. I changed back to version 3.042.008 and it started working again so something in the VB code processor got messed up in MachTurn 3.042.020.
I just spent 3 hours coding by hand a part for my Miser stirling engine. It will be made out of steel and I am a little worried about Mach not doing what is displayed. I wrote my code by trial and error, checking it in the Mach preview screen. It will be cut with a 1/8" grooving tool. I have attached it here. If you could look at it and let me know if you think it will work I would appreciate it.
Vince
-
Vince,
You were sitting right in back of me so we heard the same, but other than threading, i am not sure much has been done for turning, yet. I plan on playing around with my lathe this weekend. I finaly got it tweaked out but like you want confidence.
I am a pityfull novice code guy and just like you bought the Smid book.
Why the G53 in one of the code lines?
Attached is a DXF with some dim's ( for what it is worth ) and hopefully it represents your part, it dosn't have the curves in it.
Maybe i will turn a miniture one from your code just for kicks.
You ever consider fooling with Lazycam Turn or Lazyturn? Sure beats coding by hand!
RICH
-
The G53 puts it in machine co-ordinates so I can send the carriage to the tool change position without doing an M6.
I have tried LazyCam and LazyTurn 6 or 7 times and have never been able to get any code out of them. I am pretty good at AutoCAD and can draw up a part in just a few minutes. I would love to use that programs if I could ever get them to work. See my most recent post to the LazyTurn forum.
Vince
-
Vince,
The programs work, it's just another learning curve. Go to members docs and look thru the LazyCam Turn
manual. It's not the best, but it should shorten the learning curve. I am not going to update it since
LazyTurn is going to replace lazycam turn. It's the only writtten info that you will find.
RICH
-
Here is the DXF file for the Crosshead Guide that I spent 3 hours hand coding. It took me literally 5 minutes to draw in AutoCAD.
Vince
-
Just load up this file and see what you get, it works fine on my set-up R3.043.00
Graham
-
Below is what I got when I loaded your program into version 3.042.008. I have not tried to load version 3.043 because I am a little gun shy from my last attempt to upgrade to the lockdown version .020 what killed my VB script. What program/s did you use to produce the code?
Vince
-
Ok, that is just a setting in Mach3 that is making it look like that. My setup is like this :-
Graham
-
Graham, my setting are exactly the same as yours. It must be version 3.043. Well, I missed the reversed arcs in front. Thanks for the post.
Vince
-
Vince,
Check ...reversed arc's in front post.... in turn options tab.
Anytime you get those stupid crop circles that's what you need to do.
RICH
-
Thanks Rich, that was it. I'm glad I can keep my current version on my lathe. It seems every time I change I get bugs that I have to figure out. I installed V3.043 on my mill and now I get watchdog triggers several times a program.
Graham, I'm curious about the program to that generated the code. The feed rate is .0039 which would take about 2 weeks to cut at that rate. Looking over the code there is no tool I could use to cut it. I was planning on using a 1/8" grooving tool. I changed the DXF so code generated from it should work. I extended the section at the front of the part by 1/8" so that the front side of the tool will end up making the proper rounded corner.
Vince
-
Hi Vince,
what feed, speed, depth of cut & finishing allowance do you want and I will do you some code using your .125 tool, is it a ball end or a square end ?.
Graham
-
Hi Vince,
what feed, speed, depth of cut & finishing allowance do you want and I will do you some code using your .125 tool, is it a ball end or a square end ?.
Graham
It's square, a grooving tool. It's cutting steel so I am guessing 100 SFPM, and 1 IPM feed. Since I am cutting sideways with a grooving tool I was going to keep the depth of cut around .025".
Thanks
Vince
-
Try this version :-
Graham
-
Try this version :-
Graham
The code looks really nice. I should have time today to try it out. What program do you use?
Vince
-
AlphaCAM by Licom systems in Coventry England.
http://world.alphacam.com/Page.cfm/PageRef:1712
Graham
-
Looking over my tooling, I found that the only tool I had long enough was a grooving tool that had an insert of .060 instead of the 1/8". My 1/8" grooving tool only has a reach of 1.8". I went ahead and ran the code anyway. I only had one gotcha in that I forgot to change the reverse arcs on my computer that runs the CHNC. I caught it as it started to cut an arc the wrong way. I was amazed that it did not break the tool. I managed to save the part. The only section affected by the narrower tool was the top radius. I use the MDI screen to made up for the narrow tool and then finished it off with a file. Thanks for the code Graham.
Vince
-
Maybe I should be an engineer/machinist for a living now I have the hang of it. ;D ::) ;)
Graham
-
Maybe I should be an engineer/machinist for a living now I have the hang of it. ;D ::) ;)
Graham
Now that you have the hang of it, I have one more (Art is getting close to finishing LazyTurn but until then...). It is another part to my Miser engine. I am going to use a .060" parting tool, surface speed of 100 fpm and feed rate of 2 ipm. The raw stock is 1.5" diameter.
Vince
-
Vince try this code :-
Graham
-
Vince try this code :-
Graham
That was fast! It looks good on this end. I will try and get it cut today.
Thanks
Vince
-
I cut one on Friday night but screwed up the bore. I cut another one last night that came out well, just like the file. Thanks again.
Vince
-
:) 8)
Graham
-
Here is the part with the flute cut in it and the bottom milled.
Vince
-
So how manny parts to go Vince?
You know, this stuff can become addictive.
Lookin good.
RICH
-
So how manny parts to go Vince?
You know, this stuff can become addictive.
Lookin good.
RICH
I'm about half way. Most of the hard parts are done. Lot's of little things to make on my taig lathe then the flywheel. I have been trying to make one part a day, but in reality get one done in three days. I have a niece that has been visiting to I have spent a lot of time showing her the sites. The pictures are where I am at and a finished Miser engine.
Vince