I'm using a hardinge with a fagor 8025t control, when calculating dimensions and entering them into my program, I'm not getting what is should be. Is there annoying I can do so I don't have to lie to my machine and scrap parts making adjustments? Is it my tool radius? I have my tool radius set, should I have it on zero instead? Will my machine make up the difference?
I have 2 hardinge lathes with 8025t controls. On one lathe to get a radius on round stock I simply add the size of the radius to my -z and subtract it from my dia.
On the second I have to take my radius add my tool radius to my -z the double that and subtract from my x.
Is there a way I can determine which of the two my machines are programmed for? What is the difference between the two as far as creating programs goes? Is this something that can be changed? And if so will it alter any existing programs?
Any and all information is greatly appreciated as I have exhausted myself with studying the programming manual and have multiple questions with no answers!
it will turn a .75 diameter provided your tool geometry is set correctly.
will turn a .375 diameter.
Part radius + insert radius subtracted from the diameter is the correct X-starting point (for an OD radius) on the lathe set for radius programming. 2*(part radius + insert radius) subtracted from the OD diameter is correct for the lathe set to diameter programming.
Most people program in diameter. Easier to program. Simply take the diameters directly from the drawing. Less chance for errors. Easier for the operator to understand. I personally think it is worth the effort to set both lathes to diameter programming. Less confusion. When an operator walks from one to the other, he isn't always trying to remember which is which.
Plus, if I remember correctly, X-offsets work the same way as programming. A .003 offset on the lathe set to diameter programming will move the diameter .003, but will change the diameter by .006 on the lathe set for radius programming.
on the lathe thats believed to be set up for diameter programming, i have a facing program, and lets say i need a 45deg.x .05 +/- .01- in order to achieve a chamfer close to this spec here is my procedure;
1.003-.032(tool radius)-.094=.877 my program will look like this because i have no coolant and want a good finish
g0 g90 g70 g07 t01.01 s2500 m3
g1 x-.05 f.005
x1.003 z-.062 f.006
g0 z2.5 m5
First let me say I would not face down and then back up. I do believe in facing from the outside towards the center. The only time I don't is when the wall is thin enough to feed into the face, and then face up. This is seldom for the work I normally do. Using your specs, I would program it this way:
G0 G90 G70 G7 T01.01 S2500 M3
G1 X-.065 F.005
G1 X1.003 Z-.0683 F.003
G0 Z2.5 M5
.0183 is the tool nose radius compensation for a 1/32R insert at a 45 degree angle. Some manuals have a chart for TNRC for each whole degree from 0 to 90 degrees and for several different radius inserts. All you really need is from 1 to 45 degree. Just reverse the X-Z values from 46 to 89 degree.
My program would look a bit different as I always swing a radius at all corners to remove any burrs unless the drawing specifically specifies a sharp corner. A .05 x 45 degree chamfer with a 1/32R insert (I use .031) and a .005R on the part would look like this:
G1X1.03F.015 if you preferred a straight pull out move.
This would be a finish move. I would always first make a rouging pass on a chamfer this large.
Im impressed with the level of technicality in the program, when you rough with no coolant what is your g92 and g96 at? also what feed rate do you use?
when in rapid traverse what is the distance you travel from the workpiece? if i wanted to make a rough pass the g0 back for a finish could i trust my machine to not crash at a distance of .05? if this is the case i will change all my programs over to get the same effect on all my parts.
because of you and your advice of reading the manual, i have learned more about this machine in 7 months than my co-workers have since the got the machine 9 years ago! ive ordered a finish tool but, my co-workers are upset with me because of this, so im going to wait before i install it. i have a cutoff installed up to 1 inch, but i have no coolant. so im trying to find the best speed and feed to save inserts.what would you recommend?
again thank you for your help, its appreciated as always.
I have to be careful with drills/endmills because I can easily stall the spindle. Normally this is only when I am drilling out a soft collet before boring it to size. I may have to start small (say 3/8 in.), and step drill size up a time or two.
I normally set the G92 to the lathes maximum RPM unless the part is getting too hot. I'll run the G96 a bit slower than when using coolant. If I run a certain grade of insert at 450SFM wet in 316 SS, then I'll probably run it at 350SFM dry.
The funky move at the face of the part is to remove any possible backlash. I use to use the .02/.005 approach for boring bars also, but came to feel I was pushing my luck with some of our operators. I now use .01. Example:
Depending on horsepower, I wouldn't feed any faster than F.002/F.003 (I'd use F.002 to start with if the machine can handle it). Limit max RPM to about 2000/2500. Run SFM at about 50-75% of what the insert catalog suggests to start. If it looks good and isn't getting too hot, increase the SFM a little at a time (maybe 10% increase each time).