mastercam vs fadal vs g-code

[dforsythe]

One of the programmers left the create arcs on.

the tool was cutting away and made a left right thru the middle.

 

any ideas on how to force this from not hapening agian?

 

post ?

 

mmd has it turned off

 

Thanks, Damian

 

 

 

 

[ 05-12-2010, 04:41 PM: Message edited by: dforsythe ]

[nhraguy]

Try to make sure that your "maximum arc radius" is set to no more than 100.00 for the fadal machine. this is in the "Arc filter" page. I believe that it defaults to 1000.00. We have the same problem with our old Fadals. When that don't work I convert the large arc to a spline.

[Joe788]

YIKES! Looks like it kept on cuttin' though.

[dforsythe]

Our max is set to 100 and min is set to .1

 

the problem we have is using X4 and MP master will output a samll z move during an arc move.

 

Also it usually seems to be .0001 like the code shown above. I was just wondering if anyone else has seen this and found a way to prevent it.

 

and yes.......the cutter was just fine.

the part......not so much!

 

Thanks for the help

[Josh Kinney -Elite Engineering]

Why are you not using the Fadal post?

[Roger Peterson]

The fadal requires a larger move in Z to cut a helical arc move, I usually set it to .001" minimum. The real problem is that the fadal will mill a straight line from the start of the arc to the end of the arc if a helical arc move does not have enough Z travel (the .0001" you identified). Most machines will either ignore the small move or give you an arc error.

 

What version is the mpmaster post you are using? You can set the "mimimum change in arc plane for helix" in the control definition to .001". this should fix the issue.

[taperlength]

The Fadal graphics screen will save you from stuff like this. Takes a few minutes but cheaper than a new blank.

[peter.pen]

you can change circular output format

 

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

# Motion NC output

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

 

pcirout1 #Output to NC of circular interpolation

pcan1, pbld, n$, `sgfeed, sgplane, sgcode, sgabsinc, pccdia,

#pxout, pyout, pzout, pcout, parc, feed, strcantext, scoolant, e$

pxout, pyout, pcout, parc, feed, strcantext, scoolant, e$

[Gramby]

Similar things have happened to us. But the issue was our post forced in a G17 at each tool change. So if you had arc filter on and was doing 3d cutting in a previous tool then had a tool change for a finisher a G17 was forced in and Mastercam doesn't know it. It may suppose to be a g18 or g19?? It takes off in space scarpping the part. Just another idea.

[BBprecise]

I always leave the create arcs turned on. Mach. def. has minimum arc rad. at .0001, maximum at 400", but I also use the Fadal specific post. I've done passes like that before with no problems. Can you post/e-mail the whole toolpath, I'd like to put it in one of our Fadals. Also where is X-Y zero in relation to the center of the arc?

[Mjölnir]

Control Definition -> Tolerances -> Minimum change in arc plane for helix

 

I had similar problems on Fadals (32MP controls) until I set that value to .0002" minimum.

 

Edit:

 

Also, maximum arc radius on Fadal controls is 399.9999" as specified in the machines manuals.

[dforsythe]

We have had more trouble with our fadal post than the mp master over the years. The R values in the fadal post caused more gouges while surfacing ( which is pretty much all we do here) The guys on the floor do not want to run them in the other “Fadal” format. I tried to set the min change in arc plane to .001 and the line in question still post out with the small z move.

 

X0 y0 is c/l of the part.

 

We are using the mp master that was released around x4.

 

I have set the mach def to min rad .10 max 399.00 a long time ago and it helped.

We write 25-40 new programs per month here. This has only happened twice since we went to the mp master and tuned off create arcs. Even though it is rare this happens, I still don’t like it. Luckily the fadals are on their way out the door over the next 18 months.

 

Thanks for all the help

[Roger Peterson]

Send a zip to go to your reseller. If you have minimum change for helix arc set to .001" that what it should be doing.

[mkd]

Our Fatal 32MP runs in graphics fine, but gets "helical move too short" error when running as soon as the block in question is in the buffer.

i've been playing with "minimum change in arc plane for helix" from .0001 to .0002 but no help

 

only with MPmaster...?

 

thanks to the forum..

[mkd]

.0011 didn't work either

[Mike S @ S4A]

You may have to resort to supressing all helical output - i.e. - linearize it

 

part and parcel to using the Fadal control

[mkd]

thread hijack:

our Fadal post supplied from our Reseller works well, but i've been trying to switch over to Mpmaster.

i've beed having trouble with arcs:

 

current Mpmaster:

***********************************

X21.3 Z-.0944

X19.6181 F80.

G02 X19.6685 Y-5.7678 Z-.0945 I-30.8352 J-1.8402

G01 Y-7.5474 Z-.0944

***************************************

 

 

should be

***********************************

N900 X21.3 Z-.0944

N910 X19.6181 F80.

N920 G2 X19.6685 Y-5.7678 I-30.8352 J-1.8402

N930 G1 Y-7.5474

*********************************

 

what's up with the .0001" z moves as in the dforsythe's post?

i have filtering limited to xy arcs only and machine definition set this way. Also .0005" as minimum z for helix (in tolerances) but these have no effect on the NC.

this must be controlled in the PST file? but where?

thanks

[Alvaro Gil - Cimquest-inc.com]

If you are using R mode make sure you don't allow 360 deg arcs. Happens all the time.

 

I recommend breaking arcs at 180deg in IJK mode and 90 deg in R mode.

 

Might also want to run it through Cimco Edit with the purchased backplot option or a free program like NCPlot v1.3. 2.0 is better, but 1.3 has picked up many errors for me. http://www.ncplot.com/freetools.htm

[Alvaro Gil - Cimquest-inc.com]

MKD, silly question but is your arc geometry off by .0001" ???

[mkd]

i had I,J arcs set to quadrants. would 180° change the Z weirdness?

this particular problem with MPmaster on Fadal was using high speed core roughing.

 

other random gouges happen while using surface finish leftover.

 

some parts are perfect some get helical arc error and gouges on leftover passes.

[brandon b]

So has anyone found a solid answer on how to not get helical move too short alarm on fadals yet. I've been having almost every tool path that's filtered alarm at the machine .

[gcode]

If your machines have enough memory, disable helical arcs and output point to point code.

Its not an elegant solution, buts it's bullet proof

[mkd]

^^^yep.

it's NOT terribly expensive to have 4, 8 or 16 megs of program memory.

it will require a dash 5 CPU upgrade/ card if not already equipped.

PM me if you would like a reputable service tech. referral.

 

IIRC lots of filtered paths like to throw in a few tenths z move between arc moves (for no apparent reason) that freaks out that control. perhaps there is some post logic that can prevent this. I believe In-house has a FADAL post. Unfortunately this is a dragon that I've not slayed yet.

[gcode]

Have you tried bumping up the minimum arc length setting on the tolerance page of system confiig

[brandon b]

Yes I bumped min arc to .005. Also on the arc/ filter tab I start at .02 min arc. And go up from there . Right now I'm at .250 and still doesn't run.