Fadal post output

[Dave]

We have fadal machining centers running under format 2. When using a filtered scallop toolpath we often get the error "helical move to small" from the control. Any insights to overcome this would be helpful.

 

Dave

[perfecseal mankato]

same here, to get this to work you will need to edit the post under general output settings.

 

do_full_arc : 1 #Allow full circle output? 0=no, 1=yes

helix_arc : 1 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only

helix_tol : .0006 #tolerance in perpindicular plane for helix output

 

this should resolve the problem. the Fadal without

glass scales needs a .0003" - .0005" helical arc in order to work. that is why you need to have a

helix_tol of .0006

but this will only work in ver9.1 sp1 and up in

Mastercam.

[perfecseal mankato]

Dave,

forgot to add,

been using those settings for last 6 months and no

more problems with the "helical move to small"

error

[Roger Martin from CNC Software]

Dave,

 

Try adding a 'helix_tol' setting to your PST

(Firtst, check to see if it already exists in the PST, then you could just alter the setting)

 

The educated guess here is that the Z motion distance of that helix move is too small for the machine.

 

From the Post Processor Reference Guide CD ->

 

Code Example:

 

helix_tol : 0.001 # Minimum motion in the axis perpendicular to the arc for helix arc motion output.

 

Default:

 

If helix_tol is not defined in the post (PST file), the default setting = 0.0001 (for Inch mode) and 0.001 (for Metric mode).

 

 

Notes:

 

helix_tol is the tolerance setting for the minimum axis motion perpendicular to arc plane. If the minimum is not met and the move distance is not zero, the arc is broken with the arc linearize routine.

[mold100]

Hi Dave

 

Welcome to the forum, I just relocated from erie about 7 months ago.

[crazy^millman]

They hit the nail on the head. I would just ask what version are you running.

 

Crazy Millman

[Dave]

Thanks for the responses. We are running ver. 9.1 SP2. I tried alterng the post by changing to full arc output and all planes on helical arc support. In addition I added the helix tolerance of .0006". The program still brought up the helical move to short alarm. The problem is that you don't know if the error will occur at the beginning middle or end of the program and it becomes so time consuming. I thought I may try playing with the tolerance a bit more. Any other input is appreciated. For what it's worth We get the error on the FAdals whether they have glass scales or not. The machine I ran this test on does not have them and is running system 97.1 software.

[Dave]

I have been trying to change the helix tolerance. But when I compare the programs with different helical tolerances they seem to be identical. Which leads me to believe I'm not doing something right.

[crazy^millman]

Dave for now tell the post to linearize the lines to get you through this problem. Here it is in the MpFadal2 post:

code:

---

sub_level   : 1     #Enable automatic subprogram support

breakarcs : 1 #Break arcs, 0 = no, 1 = quadrants, 2 = 180deg. max arcs

arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

do_full_arc : 0 #Allow full circle output? 0=no, 1=yes

helix_arc : 2 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only

arccheck : 1 #Check for small arcs, convert to linear

atol : .01 #Angularity tolerance for arccheck = 2

ltol : .002 #Length tolerance for arccheck = 1

---

These setting will take anything smaller than .002 and make them line moves and not arc moves.

 

Crazy Millman

[perfecseal mankato]

Dave,

you also may want to check the filter settings on the toolpaths.

 

ours are set at

min. arc radius = .005

max. arc radius = 100.

 

using a 2 to 1 ratio on the filter settings.

 

also in the post I have the ltol = .0005

 

Our oldest machine is 13 years old the newest is 6 they run helical arcs in all planes just great with the

helix_tol = .0006 and

helix_arc = 1

 

How old is this Fadal that this is happening on?

 

Could be if it is real new that helical arcs may not work like the older machines.

You may want to consult an application engineer

at Fadal for some answers.

[Dave]

We have 5 Fadals the newest being a 65x35 with scales, the oldest is 8 years old no scales (40x 20)

The problem seems to occur on all machines, leading me to believe it is a post issue not the machine. Admitedly I'm not well versed in post code. But I don't believe my post has all the same info that was given by millman. I can't find the "atol" value. Do I need to add these lines to the post?

 

 

# INITIALIZE - initialize system variables and define user variables

# --------------------------------------------------------------------------

qtoolpln : no # MP386 - Enable tool plane option

qtoolopt : no # MP386 - Enable tool optimization

arctype : 2 # Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

do_full_arc : 1 #Allow full circle output? 0=no, 1=yes

helix_arc : 1 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only

helix_tol :0.0006 #tolerance in perpendicular plane for helix input

bldnxtool : yes # Build next tool table

ldrcode : 65 # Leader character dec. equiv. (fleader outputs code)

ncldr : 20 # No. of leader characters (fleader outputs code)

nobrk : no # Omit breakup of x/y & z rapid moves

omitcrlf : no # Omit CR/LF

omitrefht : no # Don't use reference height on first non-canned Z move

omitseq : no # Omit sequence no.

omitz : no # Omit first Z movement for non-canned-cycles

progname : 1 # Use uppercase for program name

scalex : 1.0 # Scaling of .NCI at input - x,y,z,i,j,k

scaley : 1.0 # Scaling of .NCI at input - x,y,z,i,j,k

scalez : 1.0 # Scaling of .NCI at input - x,y,z,i,j,k

seqmax : 9999 # Max. sequence no.

[perfecseal mankato]

Dave,

You could try the atol = .01, but do not know

if that would help. (can not remember if the mp9.18 executable uses both itol & atol). It should not matter if arccheck = 1. but the new executable may still look at this.

 

I could e-mail you my post for some comparisons

maybe there is something we are all overlooking.

Although the post I have is totally written for what we manufacture. If you want let me know your e-mail address to send it tou you.Then you could see if that makes a difference. (3 axis only)

[Roger Martin from CNC Software]

Dave,

 

code:

---

qtoolpln : no # MP386 - Enable tool plane option

qtoolopt : no # MP386 - Enable tool optimization

---

Seeing those variable definitions tells me you are using an old FADAL Post. Doesn't mean it won't work, but have you tried one of the MPFADAL posts from the MC CD?

 

Note that you would still need to add the HELIX_TOL setting as discussed earlier.

 

Question: On the Helix motion(s) the machine complains about, what is the linear distance int that motion block?

[crazy^millman]

I was loking at that thinking the same thing. I you contact your dealer they can get you the MPMASTER_FADAL post that emastercam has and it does great. If not look at the Mpfadal2 post I use it for our machines and it does great on problem here and never had a problem with these moves explained here and we do some very complexc 3d models here. I would update to the posts use in 9.1 or 9.1 sp2 and see if that helps. If you run into any problem gettign them to wor kthe way you want email me I will more than gald to walk you through it.

 

Crazy Millman