We get what looks like an excellent surface finish, upon polishing a
pattern of small triangles appears in the surface,.
and they are a 'BITCH" to get benched out.......This is nothing new I
have suffered with it for years, just getting tired of
dealing with it. MC says it's how the FADAL processes the code and
FADAL says it's how MC writes the code. I only have
FADALS and MC so I have nothing else to compare to. Has anyone else
experienced this if so what is the solution?
I have been using MC for over 15 years and about the same w/FADAL,
except for this I have been quite pleased with both.
I am currently using MC v9.1 spMR0304, my FADALS are cnc88 controls
w/ac drives (oldest machine 6years old).
thank you
Randy
When you program, what chord height (intol/outtol) are you using? Depending
on the degree of surface curvature, even what you think as being pretty fine
may still be way too coarse. I usually program (in Surfcam) at .001mm
(that's one micron) of chord height, and you can still see facetting
sometimes on lightly curved surfaces. A lot of people only calculate the
stepover, but that's only one component of the surface fineness in the
"along" direction, the chord height is the other component in the "across"
direction.
Now, programming that fine may choke your control if it's too old or not
equipped to handle the data throughput - the machine may shake or slow to a
crawl...
i wouldn't blame mastercam or the machine, it's the operator
programming mastercam.
You are obviouslly doing a surface, (perhaps a mould - and it requires
polishing) also what type of material are you milling, aluminum?
optimizing the program in mastercam is what needs to be done, there are
probably several dozen things to do, i wouldn't know where to start on
here, but that is the source of your problems.
-S
\> We get what looks like an excellent surface finish, upon polishing a
Randy
Are you using a scallop toolpath ?? They leave a triangular pattern on some
shapes. If the chordal tolerance is set too low you'll have larger
segements. If the path is curved in three dimensions, you'll get a bunch of
mini gouges. Actually all of the material should be above the theoretical
surface, so they're not really gouges but high and low points. This is much
more noticable when using small cutters, 1/16" ball and under.
The first thing you want to do is check, and set, the backlash compensation
in the vicinity of the work piece, especially the Z. Make sure you only
change the values for the "zone" that the part is in. Raise the point
(usually incremental) at which the tool starts to feed down.
Scallop toolpaths usually have alot of sudden direction changes (points of
triangles). This can cause an overshoot and the resultant drift back to the
correct path. This can be very problamtic when using G8. I haven't found a
way to use G9 for surfacing, it's too agressive. To minimize this, you might
want to try running the toolpath through the "high speed" processor (one of
the buttons in the operation manager). You can configure the toolpath to
slow down as it approaches a vertex, and speed back up until the next one.
The high speed control parameters are a bit cryptic, so you may have to
experiment. I usually use the defaults, and just change the min/max
feedrate. If you do allot of tweaking to get it just perfect, remember to
save the settings as a machine template.
CNC Software really needs to give you the option of putting a high
resolution loop or fillet at these intersections.
Good Luck
Mark
That high speed processor of Mastercam's is truly pathetic. Back in the
mid to late 80's "Acu-Carv" was doing a far superior job and it did it
during post processing, not on the toolpath itself. It's amazing how
Mastercam is allegedly the most widely used CAM program in the US, yet it
is light years behind the times.
When X comes out, I'm switching to Cimatron Elite. If I'm going to have
to learn a whole new interface, I might as well do it on a decent CAM
system.
And I concur, it would be really sweet to have a corner rounding option
on scallop toolpaths. It is much needed, especially for high speed
machines.
Maybe there's such an option in 9.1 MR0105? Our IT guy just installed it
last night and I didn't have a chance to go over any new functionality.
Jon,
Don't know, (haven't checked).There used to be quite a few, but then CNC
started including them in the product.
It can be done though.
Regards
Mark
message
it
yet
I would think that with all the MasterCAM seats worldwide that someone would
have written a C Hook to do this. Probably best if Randy (Hi Randy) puts up
a post on the MasterCAM forum.
jon
would
up
Jon,
Not a bad idea.
I just searched through the partners section on the MC website. Nothing
specific, but In House Solutions does have an add on package for "enhanced"
3D tool paths. Probably pricey though.
Regards
Mark
There's a "Mastercam Performance Pack" available somewhere (I'm not in
the mood for firing up a web browser to find out). IIRC, it's pretty
spendy. Maybe the same thing?
This is a multi-part message in MIME format.
--------------040308070507090306060000
Content-Type: text/plain; charset=us-ascii; format=flowed
Content-Transfer-Encoding: 7bit
Mark Mossberg wrote:
Mark,
Thank you .....I was hoping you would respond . Yes I am using
G8. I have tried every combination.....
. Have you seen this pattern I am referring to? I am machining
in finish, parallel the molds are aluminum.
I hate to repeat myself but I have been dealing with this for
years......I have been to both CNC and FADAL.
CNC has even written programs for me, same results. It seems
that the tighter the tolerence the more pronounced
the pattern. I recerived a email from a guy who sees the
same pattern w/his Vibrafree. The pattern was less
noticeable when I had older Fadals w/DC drives.
I'm just lookin for a silver bullit cure.....Maybe I'll have
one of the higher end's (Delcam or Work NC) give it
a try.
What I was really hoping for was someone w/ mutiple systems
and machines to say "this works" and "this doesn't...."
Randy
--------------040308070507090306060000
Content-Type: text/html; charset=us-ascii
Content-Transfer-Encoding: 7bit
<!DOCTYPE html PUBLIC "-//W3C//DTD HTML 4.01 Transitional//EN">
<html>
<head>
<meta content="text/html;charset=ISO-8859-1" http-equiv="Content-Type">
<title></title>
</head>
<body bgcolor="#ffffff" text="#000000">
Mark Mossberg wrote:<br>
<blockquote cite="midzGN%25d.162$ snipped-for-privacy@newssvr13.news.prodigy.com"
type="cite">
<pre wrap="">\> We get what looks like an excellent surface finish, upon
polishing a
</pre>
<blockquote type="cite">
<pre wrap="">pattern of small triangles appears in the surface,.
and they are a 'BITCH" to get benched out.......This is nothing new I
have suffered with it for years, just getting tired of
dealing with it. MC says it's how the FADAL processes the code and
FADAL says it's how MC writes the code. I only have
FADALS and MC so I have nothing else to compare to. Has anyone else
experienced this if so what is the solution?
I have been using MC for over 15 years and about the same w/FADAL,
except for this I have been quite pleased with both.
I am currently using MC v9.1 spMR0304, my FADALS are cnc88 controls
w/ac drives (oldest machine 6years old).
</pre>
</blockquote>
<pre wrap=""><!---->
Randy
Are you using a scallop toolpath ?? They leave a triangular pattern on some
shapes. If the chordal tolerance is set too low you'll have larger
segements. If the path is curved in three dimensions, you'll get a bunch of
mini gouges. Actually all of the material should be above the theoretical
surface, so they're not really gouges but high and low points. This is much
more noticable when using small cutters, 1/16" ball and under.
The first thing you want to do is check, and set, the backlash compensation
in the vicinity of the work piece, especially the Z. Make sure you only
change the values for the "zone" that the part is in. Raise the point
(usually incremental) at which the tool starts to feed down.
Scallop toolpaths usually have alot of sudden direction changes (points of
triangles). This can cause an overshoot and the resultant drift back to the
correct path. This can be very problamtic when using G8. I haven't found a
way to use G9 for surfacing, it's too agressive. To minimize this, you might
want to try running the toolpath through the "high speed" processor (one of
the buttons in the operation manager). You can configure the toolpath to
slow down as it approaches a vertex, and speed back up until the next one.
The high speed control parameters are a bit cryptic, so you may have to
experiment. I usually use the defaults, and just change the min/max
feedrate. If you do allot of tweaking to get it just perfect, remember to
save the settings as a machine template.
CNC Software really needs to give you the option of putting a high
resolution loop or fillet at these intersections.
Good Luck
Mark
</pre>
</blockquote>
Mark,<br>
Thank you .....I was
hoping you would respond . Yes I am
using G8. I have tried every combination.....<br>
. Have you seen this pattern I am
referring to?
I am machining in finish, parallel the molds are aluminum.<br>
I hate to repeat
myself but I have been dealing with this
for years......I have been to both CNC and FADAL.<br>
CNC has even
written programs for me, same results. It seems
that the tighter the tolerence the more pronounced<br>
the pattern. I
recerived a email from a guy who sees the
same pattern w/his Vibrafree. The pattern was less <br>
noticeable when I
had older Fadals w/DC drives.<br>
I'm just
lookin for a silver bullit cure.....Maybe I'll
have one of the higher end's (Delcam or Work NC) give it<br>
a try.<br>
What I was
really hoping for was someone w/ mutiple systems
and machines to say "this works" and "this doesn't...."<br>
<br>
<br>
Randy<br>
<br>
<br>
<br>
</body>
</html>
--------------040308070507090306060000--
On gentle curving surfaces the surface can be aproximated by
quite large triangles even at tight tolerances. These are
what you are initially seeing. Tightening your machining
tolerance won't help because whilst you get smaller
triangles the software just faithfully picks them out for
you. What you need to do is crank down the triangulation
tolerance to well below that of your machining tolerance.
There isn't a "triangulation tolerance" option available in Mastercam.
The only thing that comes close is the rendering (shading) tolerance,
and that has no effect at all on toolpaths.
Thank goodness rendering tolerance is usually pretty coarse.
You need to be able to limit their physical size somehow,
preferably adaptively so that it doesn't create loads of
them in truly flat areas.
On Wed, 23 Mar 2005 04:56:00 -0500 (EST), Nocturnal Dragon
I can't believe that no one has mentioned meta cut or filter max or
Mastercams own arc filtering software. even if you have a bunch of
small triangles in the incoming data you can filter a lot out with arc
fitting.
When I used Mastercam I also used Fadals and never saw the problem you
describe. But that was in 1996 last time I used Fadals.
Mark,
Thank you .....I was hoping you would respond . Yes I am using G8.
I have tried every combination.....
. Have you seen this pattern I am referring to? I am machining in
finish, parallel the molds are aluminum.
I hate to repeat myself but I have been dealing with this for
years......I have been to both CNC and FADAL.
CNC has even written programs for me, same results. It seems that
the tighter the tolerence the more pronounced
the pattern. I recerived a email from a guy who sees the same
pattern w/his Vibrafree. The pattern was less
noticeable when I had older Fadals w/DC drives.
I'm just lookin for a silver bullit cure.....Maybe I'll have one
of the higher end's (Delcam or Work NC) give it
a try.
What I was really hoping for was someone w/ mutiple systems and
machines to say "this works" and "this doesn't...."
Randy,
The backlash settings, and the high speed, "do" help. That's why I suggested
it. When you over shoot at the corners, the tool "can" go slightly below the
theoretical surface (depending on local curvature and direction). The tool
will then drift back on the path leaving a tapering line (gouge). High speed
processing will help here. Also, Fadal doesn't normaly survey the Z
ballscrew, just the X-Y. Setting the Z backlash at the height of the cut
helps here. I had all the axes re-surveyed a couple of years ago, and that
helped too.
Your right about the AC vs DC servos. The AC's are much touchier, and get
out of adjustment quicker. Open your Fadal maintenance manual (mine is 1998)
to section 4.8 "master feed rate clock". Go through the proceedures through
section 4.17 "position loop gain adjustment". I do this about every three or
four months. Takes about an hour at most, and tightens up the electronic
side of the problem.
The fault is both the code (sharp direction changes) and the Fadal. Both can
be fixed enough to give you better results
I know it's not a silver bullet, but it's what I do. I make alot of aluminum
molds with small features too.
Regards
Mark
What cut and filter tolerances are you using? My roughing tolerances are
usually 15-20% of the amount of stock I'm leaving and my finishing
tolerances are between .00005" and .0002" with 1:1 filtering depending on
the size of the work which affects compute time. I rarely see "faceted"
surfaces and when I do it's usually from a crappy imported model and re-
creating the surfaces in question solves the problem.
I agree with the Dragon on this even though I use Surfcam. The
tolerances is the biggest determining factor in surface finish. We cut
aluminum molds 90% of the time with very little polishing needed if you
use the right combination of cutter size, scallop or step over, and
surface tolerance. Loosen up the tolerance even with a very small
scallop or step over and you will get exactly what your describing.
Like Dragon says, crank the tolerance down to at least .0002. Your
program files will get huge, the computer will have to work for an extra
3 seconds to generate the program, but who cares if it will save you
time at the bench unless your machine slows to a crawl crunching all
those numbers. Then the extra time at the bench may be worth it if you
can free the machine up doing the next operation, that's something only
you can determine.
I really don't think it's the machine unless there is a serious backlash
problem someplace and that would have showed up in other places as well.
Wayne
You should think about buying a machine with a better servo system in it.
It might be more expensive initially but you'd save a lot on the benchwork.
Take a look at this link:
http://www.fanuc.co.jp/en/product/cnc/30i31i32i/nanocnc/nanocnc.html
I would give some tools, a program and some aluminum to you're local
Kitamura dealer and have them do a test cut. Then you'll see if it's in the
code or in the servos. My bet is on the servo system. The machine dealers
are usually willing to do test cuts if they think it will help them sell
you something.
Dan
Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.