Generic fanuc 5 axis post help

[DavidB]

Hi

I have been trying to resolve this problem for a few months now.

 

My problem is the Generic Fanuc 5-axis post does NOT output Unclamp and Clamp codes for DRILLING ops.

 

Every other toolpath works fine its just the drilling ops that do NOT give Unlamp and clamp codes for the Rotary Rotary.

 

I have contacted my reseller and I'm at a loss and how to get this matter resolved.

 

Inhouse said they do not support this post.

 

 

Any help appreciated

[cadman2112]

David,

 

This might be part of your issue here

code:

---

if use_clamp & not(opcode$ = three | cuttype <> zero),

[

p_lock = zero

s_lock = zero

pbld, n$, s_slock, e$

pbld, n$, s_plock, e$

]

---

In the generic Fanuc 5AX the locks come out of the checks, it check ofr an if the opcode$ equals 3, if it does it skips it, opcode3 is all of your drilling cycles.

 

That's why you are not getting it.

 

You might try changing the lines to this

code:

---

if use_clamp | cuttype <> zero),

---

That will remove the check for the drilling opcode.

 

Check it carefully though

[DavidB]

Cadman,

Your correct thats the problem.

 

I dont understand why the post would be setup to NOT clamp for drilling ops only.

 

The way I got around this before was.

code:

---

   #if use_clamp & not(opcode = three | cuttype <> zero),

if use_clamp,

[

p_lock = zero

s_lock = zero

pbld, n$, s_slock, e$

pbld, n$, s_plock, e$,

---

I would like some feed back from post gurus if this is the best way to get around the unclamp,clamp issue with drilling ops.

 

Someone must have noticed this before and have a fix.

 

Or is everyone doing there drilling ops with the rotaries unlocked?

[Bruce Caulley]

Our posts are Inhouse posts so I don't know if they are based on the same thing. We don't use the lock unless we really need it as it slows down the cycle times. If we do need it for say drilling a big hole a fair distance from centre of rotation then we add it with a manual entry.

 

Bruce

[Colin Gilchrist]

Hi Dave,

 

A little insight into what is going on here. The post is checking some boolean conditions to determine if you want to output the lock/unlock codes or not. I'm going to break it down line by line.

 

code:

---

 

if use_clamp & not(opcode$ = three | cuttype <> zero), <---- This line "says", If [the "use_clamp" variable switch is set to on] and [opcode$ does not equal 3 OR cuttype (Is NOT) zero], THEN (thats what the comma implies) STATEMENT

 

 

[

p_lock = zero

s_lock = zero

pbld, n$, s_slock, e$

pbld, n$, s_plock, e$

]

 

---

The statement in this case is an implied post block which basically just means "[Do this now]". It will execute the commands inside the braces in order without jumping.

 

I would change the code to this:

 

code:

---

 

 

if use_clamp & not(cuttype <> zero), <---- This line "says", If [the "use_clamp" variable switch is set to on] and [cuttype (Is NOT) zero], THEN (thats what the comma implies) STATEMENT

 

 

[

p_lock = zero

s_lock = zero

pbld, n$, s_slock, e$

pbld, n$, s_plock, e$

]

 

 

---

This will make sure that the rotary axes are not locked during a rapid move (cuttype = zero).

 

FYI The double less than/greater than symbols together means "Is NOT EQUAL too" ( <> ).

 

Hope that helps. By the way, I figured out all this post stuff on my own by reading the Version 9 Post Reference Guide. It is one of the most useful books I have ever read for Mastercam.

 

[DavidB]

Thanks for help guys.

Colin thanks for the explanation.

 

I should have just posted here two months ago

[DavidB]

I got this solution from my reseller

quote:

---

I would not recommend his current solution if he wishes to use this post to do 5-axis simultaneous. Simply leaving “if use_clamp” will result in unclamping and clamping every time a rotary axis repositions. Tell him to replace this:

 

 

 

if use_clamp & not(opcode$ = three | cuttype <> zero),

 

 

With:

 

 

 

if use_clamp & (cuttype = 0 | opcode$ = three | opcode$ = 16),

 

 

This will allow clamping and unclamping for tool plane positioning (i.e. 2D contours, pocketing, etc), 2D drilling and 5-axis drilling while not allowing it for 4-axis or 5-axis simultaneous movement.

 

---

Paul Decelles at CNC

[Mike-T]

*** WARNING ***

Long term use of the Forum may result in questions being answered before you get a chance to ask them.

 

Thanks guys.. just what I was looking for.

[MIL-TFP-41]

code:

---

 if use_clamp & (cuttype = 0 | opcode$ = three | opcode$ = 16),

---

if I am looking at this correctly, this will work for clamping only, not for unclamping for a 5 axis move. it also looks like that the "opcode$ = three"

can be eliminated...reason being...

 

cuttype = 0 is a flag that says it is working on tool plane possitioning, which "regular" drilling (opcode$ = three) cycles are. opcode 16 is 5 axis drilling, so the above line says its ok to clamp on 5ax drilling, which is what you want.

 

what I am trying to get around is this...Right now for a unclamp I have this

code:

---

      if use_clamp & cuttype <> zero,

[

p_lock = zero

s_lock = zero

pbld, n$, s_slock, e$

pbld, n$, s_plock, e$

]

---

Problem is having this with your clamp line could lead to extra unclamping and clamping at the first of a toolchange.

 

Also, I added another unclamp move here

code:

---

ptlchg0$         #Call from NCI null tool change (tool number repeats)                        

#Cancel check in case missed in ptoolend

if prv_n_tpln_mch <> n_tpln_mch, pg69

 

##### Custom changes allowed below #####

 

comment$

 

# This call to 'pcan' has been commented out to avoid

# double output of canned text

#pcan

pbld, n$, sgplane, e$

pspindchng

pbld, n$, scoolant, e$

if use_clamp & cuttype <> zero, ###added unclamp

[

p_lock = zero

s_lock = zero

pbld, n$, s_slock, e$

pbld, n$, s_plock, e$

]

---

I did this in case I am cutting in 3 + 2 mode, then with the same tool I do a 5 axis cut. Without this extra unclamp it will go into 5 axis mode with your clamps still on