Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Aegir on March 31, 2014, 12:31:38 AM
-
OK,
I am new, but with help from this site I am up and running on the mill. Sure, I have a long way to go, but I have made some small practise parts and am on my way, So thanks all.
Where I am having trouble now, is the lathe.
I am using Onecnc, and its not mine, but I can get access to it two or three times a week. I think I will buy it though, as I am liking the ease of use. (for the mill)
So as I am having issues on the lathe, I decided to keep it simple.
Now I realise there is no Mach 3 post in Onecnc Lathe Expert Xr5, but the mill works on either default or its Mach3 for the post.
I have tried ''default'' and ''Fanuc'' on the lathe, both as ''Tap'' and ''Text'' files, and all four do the same thing.
The round bar is 29.6mm and the tool path simulation shows it pass over at 29.6mm, for a length of 100mm . I have tried to zero Z and X on the start edge of the bar, then ''cycle start''
It goes out to X38 Z4.2 and starts in so slow, that it feels like it will never get to the next line. I have not checked jog boxes or such, as I am really trying to work out why it will not go to the stock.
When it gets to line N200 it is about 80mm approx off the bar (have not meausered that exactly) when it then runs the Z-100 pass.
I tried then to instead of zeroing on edge of the stock, I told it it was Z0 and X29.6.
To save time, I edited line N190 at gave it a value of X30, and the end result was the same as the first.
It is just a test, so not trying to cut anything. Here is the code.
Anyone know what I am doing wrong?
%
O0000
N10 (PART - )
N20 (FILE - G:\TEST LATHE.XFA)
N30 (AUTHOR - DEFAULT USER)
N40 (GROUP - TOOLPATH GROUP #1)
N50 (POSTED - MONDAY, MARCH 31, 2014 12:13)
N60 (CREATED - MONDAY, MARCH 31, 2014 09:23)
N70 (SYSTEM - ONECNC-XR5 LATHE PROFESSIONAL - VERSION 30.43)
N80 (NOTES - NONE)
N90 G00 G40
N100 G28 U0.
N110 G28 W0.
N120 (OD ROUGH RIGHT 85 DEG .8 TIP)
N130 T0101
N140 G99 G96 F0.8 S60
N150 G50 S2500
N160 M03
N170 G18
N180 G00 X38. Z4.2
N190 X35.6
N200 G01 X29.6 F0.8
N210 Z-0.8
N220 Z-100.8
N230 X38.
N240 G00 Z4.2
N250 (END TOOL)
N260 M09
N270 G28 U0.
N280 G28 W0.
N290 M05
N300 M30
%
-
While I am waiting for some input, I have been trying to offset the work piece by 29.6mm, but same result almost. It appears a little closer though.
-
You seem to be feeding at 0.8mm/min so no wonder things are slow!
Sent from my iPad using Tapatalk (http://tapatalk.com/m?id=1)
-
You seem to be feeding at 0.8mm/min so no wonder things are slow!
Sent from my iPad using Tapatalk (http://tapatalk.com/m?id=1)
I see it, and will change that one now. I offset the work piece by 38mm but still does not come back to cut it.
I have edited everything and it seems to be working. Such as line N200 I put in X0 in place of 29.6 and upped the feed. But for a complex part I could not do this, so any ideas why the code is nowhere near the part?
Default post works on the mill.
The above code is what Onecnc came up with to skim a round bar of 29.6mm diameter.
-
I would suggest that you generate code for what you want to do using one of the lathe wizards and compare that
code to what you are currently using. You need to have a Mach post processor for that software else you are going to get incorrect code for use by Mach. Fanuc had different and additional gcode as compared to Mach3 Lathe code; IE G28, G96,so have a look at the Mach3 Lathe manual for it's explaination of commands.
A few comments below:
N90 G00 .... a rapid to where?
N100 G28 U0.......see the manual
N110 G28 W0...... see the manual
N120 (OD ROUGH RIGHT 85 DEG .8 TIP)
N140 G99 G96 F0.8 S60......there is no G96 in Mach3
Since your using a subroutine we don't know the initial state of the machine / where your coming from.
Don't say if you have switches or not but will say you should touch off properly, set home, and create an offset.
Enjoy the learning experience,
RICH
-
I would suggest that you generate code for what you want to do using one of the lathe wizards and compare that
code to what you are currently using. You need to have a Mach post processor for that software else you are going to get incorrect code for use by Mach. Fanuc had different and additional gcode as compared to Mach3 Lathe code; IE G28, G96,so have a look at the Mach3 Lathe manual for it's explaination of commands.
A few comments below:
N90 G00 .... a rapid to where?
N100 G28 U0.......see the manual
N110 G28 W0...... see the manual
N120 (OD ROUGH RIGHT 85 DEG .8 TIP)
N140 G99 G96 F0.8 S60......there is no G96 in Mach3
Since your using a subroutine we don't know the initial state of the machine / where your coming from.
Don't say if you have switches or not but will say you should touch off properly, set home, and create an offset.
Enjoy the learning experience,
RICH
The mill has switches, the lathe not.
It sure is a learning experience Rich! Unfortunately there is no Mach post processor for Onecnc lathe and I was hoping to use one piece of software.
I will do a search for a Mach 3 lathe manual, and get to reading.
I thought it might be me, just being new, or maybe someone knew of a post processor that worked in place of Mach 3. Maybe a refresh on the setting home and creating offset might be best
-
Can you please attach your lathes xml.
With regards G96, in Mach, it is CSS, it doesnt work correctly (with G95) but it does work to a certain extent, ie the spindle speed will increase but the feedrate will stick at a constant feed per min rather than feed per rev as it should.
I am thinking the G96 may be your issue and seeing your xml would let me see more quickly how your lathe is set up rather than having to ask you many questions.
Hood
-
Can you please attach your lathes xml.
With regards G96, in Mach, it is CSS, it doesnt work correctly (with G95) but it does work to a certain extent, ie the spindle speed will increase but the feedrate will stick at a constant feed per min rather than feed per rev as it should.
I am thinking the G96 may be your issue and seeing your xml would let me see more quickly how your lathe is set up rather than having to ask you many questions.
Hood
Sorry, time difference and late shift.
This should be the one
-
If that is the correct profile then it is not a lathe profile. Reason I can categorically say that is the screenset you are using is Tool Setter 3-4 axis.set.
It is the screenset that defines whether it is a mill or lathe profile, if the screenset is a .set then it is a mill one (plasma etc ) for a lathe the screenset has to have a .lset extension.
Hood
-
If that is the correct profile then it is not a lathe profile. Reason I can categorically say that is the screenset you are using is Tool Setter 3-4 axis.set.
It is the screenset that defines whether it is a mill or lathe profile, if the screenset is a .set then it is a mill one (plasma etc ) for a lathe the screenset has to have a .lset extension.
Hood
Sorry about that.
That should be better
-
Ok a couple of things.
First you are in G94 (feed per min), lathes tend to be used in G95 (feed per rev)
Because of that your feedrate of 0.8mm is per min rather than per rev. 0.8mm per rev would actually be quite fast if in G95 but is deadly slow in G94, normally something in the range of 0.25 to 0.35mm/rev would be the norm for G95 for roughing.
Another thing is as Rich mentioned your code has U, V W, in Mach the other axes are A B C. Not that that really matters as they will be ignored.
There is G50 S2500, that is likely meant to limit the max RPM when in CSS (G96) but in Mach it is G48 that does that.
I would suggest you set your CAM to output as constant spindle rather than Constant Surface. Also edit your PP so it outputs a G95 and further that it will output a G48 rather than a G50 If indeed you do intend to stick to CSS (not recommended)
Hood
-
I was following a tutorial on Onecnc, and followed their settings.
I will look at the feed.
I will change it so its RPM, and edit the PP as you mention, and see how it works then.
Thanks