[jhartleyjr]

I cannot use my tap cycle on my vertical mill. When I do, the mill ignors the feedrate command on following operations and the feedrate is very very fast. See the partial post below:

N2198 G21 S4244M3
N2199 G95G84X-308.102Y-12.497Z-12.25R2.5F1.
N2200 G80
N2201 G0Z3.
(tool change)
N2202 G90 X0.Y0.
N2203 G30G91Z0T2 M6
N2204 G90 G54 X0.0 Y0.0 S9022M3
N2205 G43H2 Z1.587 G21
N2206 X-420.009Y-54.597
N2207 G1Z-1.75 F572.7
N2208 G0Z1.587
N2209 X-423.184Y-72.403
N2210 G1Z-1.75 F572.7
N2211 G03X-373.503Y-122.084R49.681 F1500.
N2212 G1X-39.603Y-122.087
N2213 G03X-34.015Y-116.499R5.588
N2214 G1X-34.016Y-10.501

Even though the G80 should cancel the caned cycle, I still have a feed rate problem on the code afterwards.

Any suggestions is appreciated.

Thanks,

John

[psychomill]

Metric program...

So you're saying when you tell it (in your program) to go "F572.7" ... it's actually feeding faster than that?
Of course, your first XY move is in rapid at line N2206
... then you have a feed jump at N2211 to "F1500."

It looks good... Is it at N2206 that you're having a problem with?

[dcoupar]

N2199 has a G95 for Feed Per Revolution. It appears to still be active when the machine reads N2210 (I don't see a G94 anywhere).

[Superman]

dcoupar is correct !!!!

It's nice to tap using the G95 code (feed per rev),

but set yourself up to cancel after any tapping by putting in a G94 ( feed per minute )

Note,,you can use a G00 in place of G80
Some machines turn the spindle OFF on G80, where G00 would only cancel the cycle

N2198 G21 S4244M3
N2199 G95G84X-308.102Y-12.497Z-12.25R2.5F1.
N2200 G94
N2200 G80 ( or G00 )
N2201 G0Z3.
(tool change)
N2202 G90 X0.Y0.
N2203 G30G91Z0T2 M6

[psychomill]

Good catch Coupar... didn't think about G95/G94. Many controls won't change feed state from G80 (or go back to default)... but....

I'm surprised your machine still feeds in G95 like that. Most controls would freak out if you're feeding at 572.7mm per revolution. That means at your toolchange, your next tool is wanting to feed at 5,166,899.4mm per minute. Can't say that I've seen too many machine that can do that .... exactly none for that matter. If it is trying to do that and the control is simply allowing it to run at max feed then something else isn't set right in the parameters.

Many tool change macros will also have a G94 in it to cancel IPR... but I have seen a few where the macro will change the status back to what ever was set prior to toolchange.... It it's G94 it goes back to G94... if it's G95, goes back to G95... G93 back to G93 , etc,etc

[jhartleyjr]

Thanks guys. That was the problem, or must have been since it has been working fine since I added the G94.

(Late thanks due to travel and inability to get logged on.)

John

[gbowne1]

I'm not that familiar with G94 & G95. I manually MDI'd a test program similar to the one posted above, and it works pretty good. I have the 0M-C, not the i version. I also had the 0M-B that I upgrated from.. I remember that the 0M-B did not work as well as my new C does with this type program.

I have the 0 control C version FANUC manuals.

Can someone explain to me the G94 & G95 codes better than the manual does?

Greg

[Superman]

Hi Greg,

G94 = Feed in units per minute
G95 = Feed units per revolution

Typically,
Lathes are normally programmed in G95 so if a feed is commanded as say F0.005" per rev. then if the spindle RPM is altered ( by program or spindle over-ride), then the feedrate is unchanged. Usually the feedrate is calculated to give a desired surface finish and the spindle RPM is calculated to suit the work material.

Mills, or milling operations are done with G94, the feedrate and RPM are not tied to each other, when setting a program up on first part the operator can tweak the RPM to suit the tool, material etc and can also fiddle with the feeds to really speed things up.Tapping on the other hand needs the RPM and feeds to link together and is done by the tapping cycle. Yes you can program a tapping cycle with G94 or G95

take this example, a 6mm x 1.0p tap
and alter RPM to S500 then to S750 ( change required is in red, blue is original )

G94 usage

G0 X0 Y0
S1000 M3 S500 S750
G43 H1 Z10.
G94
G84 Z-20. R3. F1000. M98  F500. F750.
G80

G95 usage

G0 X0 Y0
S1000 M3 S500 S750
G43 H1 Z10.
G95
G84 Z-20. R3. F1. M98
G80
G94

Note!! When using G95, the tap cycle is fixed to the pitch required, it also eliminates the calculation mistakes that can happen, as the feed is the thread pitch, and does not relate back to the RPM.

The real issue to watch out for is, you must cancel the G95 after tapping

[davisboys]

I always tap in G94. I don't get what is the benefit of tapping in G95? Clearly you must change back to G94 after using G95.
I choose a feedrate....say F50. Multiply it by the TPI and arrive at RPMs. Never have been able to fault the machine or control for tapping problems.

[gbowne1]

I've never done machine tapping before, but I have tried the cycle from a macro. But, in a recent CNC training class I took, I got a chance to do some 0T threading on an OD part 8tpi on a laydown. In my 0M-C I have both the 1mb memory cassettes so I have quite a lot of macro / memory. I just had to try out a program smiliar to yours to see if it works. I always pay attention to command structure in G Coding and aware of cancelling things to return to normal operation.

As an aside, Building FANUC controls from parts off eBay is cool but you gotta get the right part numbers. I built my 0M-C from scratch. Cost me a arm and a leg but I like this one far better than my 0M-B. The C version CRT/MDI was hard to find and not real cheap either. Most things ended up to be less than a grand each.. but I've gotten lucky some times. Glad I had the manual set for the 0M-C. If you don't have one, get access to Al_The_Man's divshare for the 0MC manuals. One of them is like 900+ PDF pages.

I used to have a chart which showed general speeds and feedrates in both metric and inches/SAE for many different materials. I use a lot of 4100 and 4300 series moly/chromoly steel.. and I've built my own table based on experience with lots of those. I also do a lot of 2024, 7075, 6061 aluminum types different -T numbers, different hardnesses, annealed and hardened. It pays to pay attention to speeds and feedrates and not try and overdo it. I always start with your minimums and work up from there till it starts cutting at the desired results. Too slow or to too fast you can really wreck somethin' and I know you'll not want to crash. If anyone wants my charts they are in Excel / OpenOffice 3.0 Calc.

Greg