Inch feedrate help..........

[Lstar]

i have some former program using feedrate in inch(most of time i use MM feed), the NC program doesn't call G94 in the beginning and the feedrate for milling are not without a decimal point, that is "F100" , it move very slow when i run it, then i have try to add G94 in front of it ,but its still move very slow, it seem only 1 inch per minute (not 100 nich). unless i change all of the F*** to F***. then i only have the right feedrate. i think it should have some other setting for G94. please help.

[Lumpnut]

Not quite sure I understand your question , but I believe you have to have a decimal in the feed rate callout... ex. F100. , whether you use G94 or not.

[Tim Johnson]

On a Fanuc you don't need the decimal point but F100 would equal F.1 per minute, X-50 equals X-.005. ect.

 

HTH

[Lstar]

they run this program in their shop with no problem, all of the feedrate are without decimal point. but i can only get in seem 0.1 inch per minute. maybe there is a parameter setting , but i don't know it. what are the F51 F52 setting for G94?

[Tim Johnson]

What control was this programmed for and what control are you using?

[Lstar]

fanuc 16iM .

[Storkman]

quote:

---

F100 would equal F.1 per minute

---

Use F10000 to get F100.

 

Our old Rambaudi 4 spindle used to read code like that.

[mcpgmr]

Try G20 in begining. It's Inch mode. G94 only changes from IPR to IPM or cancels G93 Inverse feed. HTH

[steelersfan]

Have run into same problem myself on fanuc 18m control. I added decimal point to feedrate to correct. Jerry

[Storkman]

Welcome Jerry, sorry you were pinned with that screen name.

 

 

 

 

[Lstar]

quote:

-----------------------------------------------

Use F10000 to get F100.

-----------------------------------------------

so i have to change all of the feedrate in my program, it is a long program, i think it would be the same to add all of them with decimal point.

 

 

quote:

-----------------------------------------------

Try G20 in begining. It's Inch mode............

-----------------------------------------------

i have tried this before i post this question,not function

[Lumpnut]

quote:

---

so i have to change all of the feedrate in my program,

---

Is there a find and replace function in your control??? ex. find F100 / replace with F100.

 

That might speed things up for ya. Just a tought.

[Tim Johnson]

quote:

---

What control was this programmed for and what control are you using?

---

quote:

---

fanuc 16iM

---

There are no parameters shown in the fanuc manual.

Are you sure that the control that the program was originally made for is fanuc?

[heeler]

I think that you can look at Parameter #3401 bit #0 DPI When a decimal point is omitted in an address, the least input icrement is assumed (0)/ The unit of mm, inches, or sec. is assumed (1). We have ours set at (1) and input feeds without decimals all the time.

 

HTH

 

Glenn

 

P.S. This is from the Fanuc Operation and Maintenance Handbook

[Tim Johnson]

Thanks Heeler,

I looked in the operators/ programmers manual.

[Müřlıń®]

Change the format statement in your post and it will be done for you when you run the post

[Storkman]

quote:

---

so i have to change all of the feedrate in my program, it is a long program, i think it would be the same to add all of them with decimal point.

---

if you use the MCEDIT editor, you can scale up or down any factor. Just multiply all the "F"s by 1000.

[Storkman]

What did you end up doing Lstar?

[Lstar]

Thanks all of you guy.

quote:

------------------------------------------------

I think that you can look at Parameter #3401 bit #0 DPI..........set at (1) and input feeds without decimals all the time.

 

------------------------------------------------

Thanks heeler. may it effect the tapping cycle G84? anywhere i will try it later.

 

 

quote:

------------------------------------------------

Is there a find and replace function in your control??? ex. find F100 / replace with F100.

 

------------------------------------------------

Yes, but i have not only F100, they are F30 F50 F80 F100 F200. i can change them in the editor.

if not found good way, next and next inch program, they may need to be change in the editor

[Lstar]

Thanks Tim Johnson.

 

quote:

------------------------------------------------

There are no parameters shown in the fanuc manual.

Are you sure that the control that the program was originally made for is fanuc?

------------------------------------------------

 

they told me that they run it in other control, but all of the G code are the same. so i think there would not have big difference . there must have the switches in all this control that runing in the G code same as Fanuc

 

[sammgujjar]

my dear whats ur controler name

and in some cases the f rate is can not be change with g94 ... u use the MM with g94 but if ur rate can not be change plz send me us nc controler name and spacifection i help u beter then now..

[Lstar]

quote:

------------------------------------------------

my dear whats ur controler name..............

plz send me us nc controler name and spacifection i help u beter then now..

------------------------------------------------

 

sammgujjar please read from the beginning

[Tom Dorgan from American Precision]

Try a G70. Some controls use a G20 and others a G70 for inch moves. Should not matter if you have a decimal or not but I prefer them because when editing it deliniates between F200 and F20 for example.

[pip]

Maybe the feedrate is in Inch/mm per revolution G93, and that's why it's not working correctly.

Just a thought.

[heeler]

quote:

---

Thanks heeler. may it effect the tapping cycle G84? anywhere i will try it later.

---

We use the G84 with a tapping head, and with a rigid tap setup and have had no problems.