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).
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...
\> 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.
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.
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.
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.
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 Fedo wrote in news:MIidnS48X-z26qLfRVn-jA@t- one.net:
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:
formatting link
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.
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.
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.
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.
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.
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?
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.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.