Why do I have to remove all the G94 lines??

[paynebros]

I am using a few different programs through school such as Feature Cam,and when I load in the program I get an error every time and when I remove the G94 line it works fine . Normally this is not an issue but now I am learning to tap and I am sure that I will need this for feeds and speeds. I don't store any offset values as I have just begun to work with the machine, Do I have something incorrect Here is a small sample program segment. Thanks for any help and advice you have. Oh yeah, I have a tree journeyman using dyna delta 20.


N20G70G90
N25EE01T12M06
N30G94
N35S3162M03
N40M08
N45G00X0.5083Y0.3161Z1.0F10.3
N50G00Z0.1
N55G01X0.5083Y0.3161Z-0.0499F10.3
N60G01X0.4741Y0.3034Z-0.0499F20.6
N65G01X0.4425Y0.2996Z-0.0499
N70G01X0.4109Y0.3034Z-0.0499
N75G01X0.377Y0.3161Z-0.0499
N80G01X0.3477Y0.3357Z-0.0499
N85G01X0.3357Y0.3477Z-0.0499
N90G01X0.315Y0........................................

[jagardner4]

What error are you getting?

Also, check the EIA Assist page to see if the G94 code is listed as one of the allowable G codes. The Delta 10/20 mill control never implemented IPR feedrate (G95), so there was no reason to accept a G94 (IPM feedrate) until inverse time (G93) was implemented.

[mactec54]

paynebros

G94 are mostly used for lathes so you mill will not like them being there, You need to change your post, so they are not there, It most likely should be a G90 for absolute

[paynebros]

Thanks that make sense and I will remove it in the processor, I had some help writing a tapping line for drip feed and when I ran it it fed down correctly but when it changed directions it did a fer quick rotations ruining the threads and then retracted correctly. I am using wood to practice with for now so no harm done, but can someone help me write EIA code for a simple tapped hole using a 1/4" x 20 tap in and out. I will continue to practice with wood but I have received it several different ways now and none have completed the tap. Same Tree Delta 20 setup and Sure appreciate the help and advice!

[mactec54]

paynebros

Try this it is a simple program for 1/4-20 (3) holes 2" apart, Does you machine have a spindle encoder, if it has not then you can't Machine /Ridgid Tap like this

[paynebros]

I looked today through my manuals and could not see if it was capable but was also told to run your program and it will error out if it wont ridged tap. Thanks again for the help.

[jagardner4]

A Delta 20M will not rigid tap. The feature wasn't developed until after the Delta 20 was discontinued. Rigid tapping requires encoder feedback from the spindle so that the Z axis movement can be coordinated with the actual spindle movement.

The G84 tap cycle (or G4 in the Position Event) assumes you are using a floating tap holder.

[paynebros]

Thanks again for the continuing information. I better take advantage of the help while I have such a good broad source of information available, soooo... I have had mixed results with using the tool table page. I have been training on a mazak machine at work and have the task of pushing the start button and making all the tool offsets as they wear down. so when I tried to use this same procedure at home with my tree mill I cant get any tool diameter compensation. I have gone in to the tool table page and set the Z axis by touching off the part and hit the soft key "Set" on the panel and that works fine, but the diameter offset I manually enter into the table will not adjust at all. I use a regrind 3/4 end mill and it is .010 smaller in size . so I have tried both entering -.005 and .005 into the tool table and it follows the same path as if it was a perfect .750. Is there a line of code I need to activate the tool offset, and why will the z work but not the diameter? I sure do appreciate the feedback I have received please keep it coming!, I have learned more through this site and work then I got throughout my entire associates degree! Not that the shop teacher was bad but you could tell the years of dealing with knuckleheads has ruined the motivation he once had!

[mactec54]

paynebros

Just put the tool in at .740 & see if that will work

[Superman]

Originally Posted by mactec54 paynebros G94 are mostly used for lathes so you mill will not like them being there, You need to change your post, so they are not there, It most likely should be a G90 for absolute

????
I think this comment needs checking

lathes are best programmed using Feed / Rev ( G95 )
if you adjust the spindle over-ride control, the feedr is also adjusted to stay at the programmed rate
ie RPM=1000 F=0.01/rev
slow the spindle and the feed is kept the same 0.010"/rev

Mills are standard set to G94 ( feed / minute )
this keeps the over-ride pots independant to each other
You can use G95, but caution should be used to make sure it is switched back to G94
G95 is ideal to be used when hole making ( generally only boring or RIGID tapping )

Some machines are fixed to using G94, so it may be a code that is not allowed ??

Another option to RIGID tapping ( tap is sloidly clamped in a non-flexible holder ) is the use of a spring tapping holder, feedrate should be about 95% of the calculated feed per rev
take a metric M6 x 1.0 pitch tap


RIGID Holder ( G94 mode ) S1000 F40.00 (F= pitch X RPM )
RIGID Holder ( G95 mode ) S1000 F0.040 (F=pitch )
Tapping Holder ( G94 mode ) S1000 F38.00 (F= pitch X RPM X 95% )

[mactec54]

Superman

The G94/G95 command is modal and usually set very early in the program.

Unless you are programming a lathe and use G94 to move around the part and G95 to cut the part, it is pretty much a set it and forget it command.

Most CNC machines run boot program when they start up that sets the most common modal commands. If you are running a mill, it will no doubt default to G94 when you turn the machine on.

(You only need to look at the control screen & you will see what has been loaded in modal commands)

A lathe could default to either G94 or G95, so make sure that one of the first lines in your program always sets the initial conditions you want default to.

This is why it should not be in his Mill program,as he found out, The control did not like it being there

As for my post about this G94 being in his program, that you seem to see as incorrect it is not,

You don't put a G94 in a mill program it is not needed,& should not be there, It is only put in Lathe programs when needed, or Mill/Lathe Type machines

[jagardner4]

To work, Cutter Diameter Compensation (CDC) requires that you not only call up the desired tool diameter. but also tell which side of the cut you are on.

I think in your case, the T code indicates the diameter offset to use, so the code you've posted is okay, but there's a small possibility the parameters have been set to call tool diameters via a D code programmed in Event Type 9 (M Function Event). Check the M Function event for a D code line. If it doesn't have one, stick with calling the tool diameter by way of the T code.

Once you've called up the offset you want to use, you need to activate it and tell the control which side of the cut to put the compensation on. This is done by programming C1 or C2 in a Linear or Arc Mill event (event types 1 or 2). I don't remember which code tells the control to put the cutter to the left of path and which puts it to the right, but there will be a help message that comes up telling you which one is which. Diameter compensation remains active only while executing lines and arcs (event types 1 or 2), so programming any other event will 'interrupt' it and shut it off.

G41 and G42 are the G code equivalents for C1 and C2 in the conversational events.

There's a lot more rules and such discussed in the manual about cutter compensation. You should really take a few minutes to read the section.