G02 & G03 in MDI
- welderfabrod
- Offline
- Junior Member
Less
More
- Posts: 29
- Thank you received: 0
14 Jun 2010 19:00 #3141
by welderfabrod
G02 & G03 in MDI was created by welderfabrod
Hi guy's I'v been trying to use G03 in MDI to put a bellmouth at the start of a premachined bore.
My lathe is in radius mode.
The bore is 38.9mm. dia.. The radius of the bellmouth is 11.80mm.
The bellmouth Radius starts at X27.535 Z0. Which is where I position the cutter before commanding the G03.
The radius ends at X19.45 Z-11.20.
My centre offsets are I 3.715 J -11.20
My G03 is therefore X19.450 Z-11.200 I3.715 J-11.200 F60
But I get the error message Start=(X22.535 Y0.000), Center=(X31.25 Y-11.200) End=(X19.45 Y0.000), r1=11.8001 r2=16.269
Why is it showing Y instead of Z
Why is the end point Y0.000 instead of Y-11.200 or more appropriatly Z-11.200.
And I would have thought the centre offsets would have be in incremental i.e. X3.715 Y-11.200 not Absolute as shown or does EMC2 internally work in Absolute.
And whats wrong with my Gcode. or am I missing something here.
Thanks Rod
My lathe is in radius mode.
The bore is 38.9mm. dia.. The radius of the bellmouth is 11.80mm.
The bellmouth Radius starts at X27.535 Z0. Which is where I position the cutter before commanding the G03.
The radius ends at X19.45 Z-11.20.
My centre offsets are I 3.715 J -11.20
My G03 is therefore X19.450 Z-11.200 I3.715 J-11.200 F60
But I get the error message Start=(X22.535 Y0.000), Center=(X31.25 Y-11.200) End=(X19.45 Y0.000), r1=11.8001 r2=16.269
Why is it showing Y instead of Z
Why is the end point Y0.000 instead of Y-11.200 or more appropriatly Z-11.200.
And I would have thought the centre offsets would have be in incremental i.e. X3.715 Y-11.200 not Absolute as shown or does EMC2 internally work in Absolute.
And whats wrong with my Gcode. or am I missing something here.
Thanks Rod
Please Log in or Create an account to join the conversation.
14 Jun 2010 23:17 #3146
by BigJohnT
Replied by BigJohnT on topic Re:G02 & G03 in MDI
Rod,
Are you in the XZ plane with G18?
Also note that the G2/3 rotate about the imaginary Y axis plus end so if your setup is normal you have to lay on the floor and look up for G2/3 to seem normal.
Another thing is diameter mode... if your in diameter mode X is diameter but X offset (I) is in radius.
I was struggling the last few days on my lathe with this too.
John
Are you in the XZ plane with G18?
Also note that the G2/3 rotate about the imaginary Y axis plus end so if your setup is normal you have to lay on the floor and look up for G2/3 to seem normal.
Another thing is diameter mode... if your in diameter mode X is diameter but X offset (I) is in radius.
I was struggling the last few days on my lathe with this too.
John
Please Log in or Create an account to join the conversation.
- welderfabrod
- Offline
- Junior Member
Less
More
- Posts: 29
- Thank you received: 0
15 Jun 2010 08:00 #3150
by welderfabrod
Replied by welderfabrod on topic Re:G02 & G03 in MDI
Thanks for the reply John as I said my lathe is in radius mode. I also used the stepcon wizard to set it up so as I selected the lathe option there I thought I would'nt need a G18. But I'll give this a try today.
When this first happened I thought that maybe stepcon had failed to set it in lathe mode so I checked and its definitly in lathe mode there. I also looked at my ini. file and did notice that although XZ is there the number of Axis was still set at 3. So I tried to reduce this to 2 but when I restarted Axis it threw up an error about the number of axis so I put it back to 3.
Oh yes I did try this with a G02 as well the result was the same.
As I said I'll give the G18 a try today although I,m still unsure why I should need this as Axis should know that I'm in lathe mode and therefore surely always in G18.
Also I have run programs with G02 & 3 and have never used a G18 yet so is this something that is only needed in MDI.
Curious, Rod.
When this first happened I thought that maybe stepcon had failed to set it in lathe mode so I checked and its definitly in lathe mode there. I also looked at my ini. file and did notice that although XZ is there the number of Axis was still set at 3. So I tried to reduce this to 2 but when I restarted Axis it threw up an error about the number of axis so I put it back to 3.
Oh yes I did try this with a G02 as well the result was the same.
As I said I'll give the G18 a try today although I,m still unsure why I should need this as Axis should know that I'm in lathe mode and therefore surely always in G18.
Also I have run programs with G02 & 3 and have never used a G18 yet so is this something that is only needed in MDI.
Curious, Rod.
Please Log in or Create an account to join the conversation.
15 Jun 2010 12:13 #3151
by BigJohnT
Replied by BigJohnT on topic Re:G02 & G03 in MDI
Rod,
While the user interface Axis "knows" it is in lathe mode EMC has no such thing as lathe mode and defaults to G17 XY plane when started. While you can put G18 in your ini file that won't stop another g code program from changing it so it is always best practice to put all your setup g codes in the preamble of your program. I include a standard line similar to G7 G18 G20... as the first line of all my g code files.
Even though you only have two axis on a lathe they are 0 and 2 so you need to load 3.
I'd bet your offsets are not correct as that it the hardest thing to get right.
Just drawing your arc in ACAD and I have the following coordinates.
Arc Start X27.535 Z0
Arc Center X31.250 Z-11.1999
Arc End X19.450 Z-11.200
Doing the math I get
X offset 3.715
Z offset -11.1999
So I end up with:
G8 G18 G21
G0 X27.535 Z0
G3 X19.45 Z-11.2 I3.715 K-11.200
This give me an arc of about 270 degrees... not sure your wanting that. Changing to G2 give me about 90 degrees.
Scrolling down to compare I this I see your using the XY offsets IJ instead of the XZ offsets of IK... so your math was sound.
www.linuxcnc.org/docview/html//gcode_main.html#sub:G2,-G3:-Arc
John
While the user interface Axis "knows" it is in lathe mode EMC has no such thing as lathe mode and defaults to G17 XY plane when started. While you can put G18 in your ini file that won't stop another g code program from changing it so it is always best practice to put all your setup g codes in the preamble of your program. I include a standard line similar to G7 G18 G20... as the first line of all my g code files.
Even though you only have two axis on a lathe they are 0 and 2 so you need to load 3.
I'd bet your offsets are not correct as that it the hardest thing to get right.
Just drawing your arc in ACAD and I have the following coordinates.
Arc Start X27.535 Z0
Arc Center X31.250 Z-11.1999
Arc End X19.450 Z-11.200
Doing the math I get
X offset 3.715
Z offset -11.1999
So I end up with:
G8 G18 G21
G0 X27.535 Z0
G3 X19.45 Z-11.2 I3.715 K-11.200
This give me an arc of about 270 degrees... not sure your wanting that. Changing to G2 give me about 90 degrees.
Scrolling down to compare I this I see your using the XY offsets IJ instead of the XZ offsets of IK... so your math was sound.
www.linuxcnc.org/docview/html//gcode_main.html#sub:G2,-G3:-Arc
John
Please Log in or Create an account to join the conversation.
- welderfabrod
- Offline
- Junior Member
Less
More
- Posts: 29
- Thank you received: 0
15 Jun 2010 19:06 #3155
by welderfabrod
Replied by welderfabrod on topic Re:G02 & G03 in MDI
Thanks John I think I understand why it needs the G18 now. I also posted this on CNC zone and a reply from a guy on there pointing to the error of my ways with I J sorry K did G18 G03 X19.45 Z-11.2 I3.715 K-11.2 as he suggested and everything worked fine. I also did another Gcode entering a wrong dimension in my off sets just to test it, it through the error as expected but this time had the Z axis instead of the Y. Now I just have to log it in my brain for recall later. Not an easy task at my age.
Thanks for your help Rod
Thanks for your help Rod
Please Log in or Create an account to join the conversation.
15 Jun 2010 21:04 #3158
by BigJohnT
Replied by BigJohnT on topic Re:G02 & G03 in MDI
I hope to soon have a morphed version of my arc buddy for lathes. If you have a mill to you might want to take a look at it on the wiki.
John
John
Please Log in or Create an account to join the conversation.
22 Sep 2011 14:25 #13360
by piasdom
Replied by piasdom on topic Re:G02 & G03 in MDI
what's the formula to find the cut radius. i'm trying to cut a
1/4" radius with a 3/16" end mill. with a 1/4" end mill, i know it's 1/8" radius for i and j.
this is my start
g17 g20 g40 g49 g54 g80 g90 g94 g92.1
Thanks
kenneth
1/4" radius with a 3/16" end mill. with a 1/4" end mill, i know it's 1/8" radius for i and j.
this is my start
g17 g20 g40 g49 g54 g80 g90 g94 g92.1
Thanks
kenneth
Please Log in or Create an account to join the conversation.
22 Sep 2011 14:38 #13361
by piasdom
Replied by piasdom on topic Re:G02 & G03 in MDI
drawing it in cad i get .156" but i would still like the formula
as i still don't know if this is right.
Thanks
kenneth
as i still don't know if this is right.
Thanks
kenneth
Please Log in or Create an account to join the conversation.
25 Sep 2011 03:54 #13435
by jmelson
Replied by jmelson on topic Re:G02 & G03 in MDI
piasdom wrote:
3/16" end mill is .1875"
So, the 3/16" end mill needs to orbit the difference between these
sizes, which is .0625" diameter. The radius of that would be
.03125"
The way to think about it is the hole is .250" diameter.
The tool radius is .09375", and the tool center needs to
approach each side of the hole leaving a clearance of its
radius. So, simply, hole diameter - tool diameter is the
diameter of the toolpath circle.
Jon
That doesn't sound right. 1/4" is .250 diameterdrawing it in cad i get .156" but i would still like the formula
as i still don't know if this is right.
Thanks
kenneth
3/16" end mill is .1875"
So, the 3/16" end mill needs to orbit the difference between these
sizes, which is .0625" diameter. The radius of that would be
.03125"
The way to think about it is the hole is .250" diameter.
The tool radius is .09375", and the tool center needs to
approach each side of the hole leaving a clearance of its
radius. So, simply, hole diameter - tool diameter is the
diameter of the toolpath circle.
Jon
Please Log in or Create an account to join the conversation.
26 Sep 2011 10:14 #13451
by piasdom
Replied by piasdom on topic Re:G02 & G03 in MDI
thanks jmelson, but if i use that formula;
1/2" hole using 1/4" endmill = 1/2"(.5) - 1/4(.25) = 1/4"(.25) radius
i cut a lot of 1/4"(.5 hole) radii and i always use 1/8"(.125) radius to get 1/4" radius.
(below is example)
so if i sue that formula for 3/16"
1/2"(.5) - 3/16"(.1875) = 5/16"(.3125) radius.
unless i don't understand the formula (been known to happen:)
g1 x.04 y-.165
g2 x.165 y-.04 i.125
g1 x3.565
g2 x3.69 y-.165 j-.125
g1 y-.275
g2 x3.565 y-.4 i-.125
g1 x.165
g2 x.04 y-.275 j.125
Thanks
kenneth
1/2" hole using 1/4" endmill = 1/2"(.5) - 1/4(.25) = 1/4"(.25) radius
i cut a lot of 1/4"(.5 hole) radii and i always use 1/8"(.125) radius to get 1/4" radius.
(below is example)
so if i sue that formula for 3/16"
1/2"(.5) - 3/16"(.1875) = 5/16"(.3125) radius.
unless i don't understand the formula (been known to happen:)
g1 x.04 y-.165
g2 x.165 y-.04 i.125
g1 x3.565
g2 x3.69 y-.165 j-.125
g1 y-.275
g2 x3.565 y-.4 i-.125
g1 x.165
g2 x.04 y-.275 j.125
Thanks
kenneth
Please Log in or Create an account to join the conversation.
Time to create page: 0.093 seconds