Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Richard Evans on December 22, 2012, 03:36:10 PM
-
I need to turn some shallow 'inward' arcs- a bit like a file handle-- in bar stock.
I've read the Lathe Arc Motion document several times but it's pretty difficult stuff.
As an example, an arc 50mm in length from z-10 to z-60 (so G03 anticlockwise?) at a radius of 600mm in 20mm diam. stock.
I thought this would do it, assuming the cutter is already at X20,Z-10:
G03 X20 Z-60 R600
When I tried this on the MDI ( just simulation) the Z value is getting bigger (closer to zero) so something is wrong. I have ticked 'Reverse Arcs in Front Post' in the config, before that X was also getting bigger.
Any suggestions? I am probably missing something obvious, not for the first time.
Thanks for any comments
Richard
-
Try with G2
Hood
-
I've read the Lathe Arc Motion document several times but it's pretty difficult stuff.
I know what you mean and I wrote it...... :D
The document covers a lot of information and one needs to study it. Now the fun stuff was done just to show
all the different combinations depending on how the code is written for different combinations. You can just extract each part of code
and play with it . Put all together the Radius Arc Moves code just does a bunch of moves going one direction and then back.
No wonder I decided to just buy a lathe package. ???
I like Newton's viewpoint.....if one can write it done on a piece of paper why keep it in your egg / head......well not quite a qoute but you get the gest! ;)
RICH
-
This seems to do the trick:
G18 G21 G40 G49 G64 G80 G90 G94
G0 X0 Z0
G1 X20 F200
G1 Z-10
G2 X20 Z-50 R100
G1 Z-30
This was done by substituting my values into one of the routines at the end of the Arc Motion document, also same as Hood's suggestion. However it only works with the 'reversed arcs in front toolpost' box unticked in Config. This is a bit of a pain because I have other arc routines written with the wizard and I think they won't work now. However, it would be easy enough to change the config when I need to use those routines.
The important thing is that having got something to work, I can play about with the other sample programs knowing that I have a fallback position.
So, thanks to Hood and Rich, not for the first time!
BTW Rich, I would buy a lathe CAM package but I actually work in wood (making bagpipes) and much cutting is done using a parting off tool, using the sides of the tool in both Z+ and Z- directions. This would make any metalworker wince and is not catered for in any normal CAM package!
Cheers
Richard
-
This would make any metalworker wince and is not catered for in any normal CAM package!
Not at all, there are tools specifically meant for grooving and turning, normally called MDT (Multi Direction Turning) tools. I have one from Seco and use it at times for odd shapes.
Heres a tool path showing one being used in Dolphin.
Hood
-
And here is the toolpath it would take.
Hood
-
Richard,
LazyTurn is free, has a manual / is documented, and does outside profiles. Have a try as it may just do all you need to do.
As far as the tool is concerned you can create a parting tool and define what side the cutting edge is.
You need to pay attention to the figures in the Arc Motion write up. Figure 9 captures what can influence the generated G code.Figure 16 provides a visual as to g2 / g3 motion for front and rear tool post. Thus a lot of combinations and different motion.
RICH
-
BTW,
Once you have the shape done, and if you have a drilling device which you can install on the carriage, then you can drill holes using the lathe macro drilling cycles, thus not have to remove the pipe from the lathe.
Just a thought,
RICH
-
This would make any metalworker wince and is not catered for in any normal CAM package!
Not at all, there are tools specifically meant for grooving and turning, normally called MDT (Multi Direction Turning) tools. I have one from Seco and use it at times for odd shapes.
Heres a tool path showing one being used in Dolphin.
Hood
Didn't know that- that's really what I'm doing with a parting tool sharpened down the sides. I have a demo of Dolphin but I can't get into it somehow, it's faster to write the fairly simple code by hand. I use Sheetcam on the mill and am more or less OK on that.
Cheers
Richard
-
Richard,
LazyTurn is free, has a manual / is documented, and does outside profiles. Have a try as it may just do all you need to do.
As far as the tool is concerned you can create a parting tool and define what side the cutting edge is.
You need to pay attention to the figures in the Arc Motion write up. Figure 9 captures what can influence the generated G code.Figure 16 provides a visual as to g2 / g3 motion for front and rear tool post. Thus a lot of combinations and different motion.
RICH
Lazyturn would do what I want but for some reason the post isn't working, it just produces an empty file. I'll take another look.
The Arc Motion doc. is great, I just need to go very slowly!
I'm making all these bits by hand right now, but it's catch-22- CNC is much faster but I have to stop making stuff to teach myself, and time is short.
Cheers
Richard
-
BTW,
Once you have the shape done, and if you have a drilling device which you can install on the carriage, then you can drill holes using the lathe macro drilling cycles, thus not have to remove the pipe from the lathe.
Just a thought,
RICH
Thanks for the suggestion! I have a very nice cnc milling machine which does this job, and a lot more, using Sheetcam.
Cheers
Richard
-
Hi,
What settings do I need to use the "R" value for radius's in Mach 3 lathe?
I noticed you guys were using "R" value. I've tried G2 & G3 with R and I am still getting funky arcs.
-
You would have to attach your xml and code to really see where things were wrong.
Hood
-
I have tried both G2 and G3 with the "R" value and gotten bad arcs. I don't perfer to use I&K. What settings in Mach do I need to change to use the R value for radius?
-
As said if you attach your xml and code the problem may be found.
Hood
-
Coolant Slinger,
What settings in Mach do I need to change to use the R value for radius?
Study the figures in the Mach3 Turn - Arc Motion write up. Page 12, 15-17. Question as posted is ambiguous.
RICH
-
Here are the files
-
Ok not really sure exactly what things are meant to look like but could you have the arcs reversed? If you go to Config menu then Ports and Pins then finally Turn options und take the tick out of Reversed Arcs in front post does it look OK?
Hood
-
Coolant,
Using your the first part of the code only, Mach shows arc's here with Reversed arc's unchecked, absolute and diameter mode,
else you will get crop circles.
RICH
-
Hood,
You were right I removed the tick out of Reversed Arcs in front post and my arcs came out good.
And Thanks to Rich also.