Build 6903
April 3, 2008 · Filed Under MeshCAM Development
I just posted a new build to http://www.grzsoftware.com/files/MeshCAM2-6903.exe . It includes new waterline and pencil code that will hopefully address some of the problems that people have mentioned. In my testing it seems better in every case I’ve tried. There’s still room to improve but I will be curious what to hear what others think.
Comments
23 Responses to “Build 6903”
I just tested 6903, The parallel finish misbehaves when used with waterline and a tapered end mill. You can reproduce this by loading a STL of a cube-2×2x2, stock-3×3x3, make positive X&Y, top-of-part-zero, X&Y centered, generate a tool path for it using an end mill with a tapper less then 12 degrees. You will see that the parallel finish feeds up and down two sides of the part. Interestingly enough I was also able to make the parallel finish misbehave in this fashion with a non tapered end mill that had a flute length less then the max depth. More info and pictures are in the meshcam yahoo group.
Best Regards
DAG
Playing with a 2×2 mm cube, stock 5×5 mm, machine entire stock. Just finishing looked fine but when combined with a waterline just the model was finished not the stock. The finish also does not always go to the full Z depth. The problem goes back a few builds, 6838 was the last one which didn’t have this problem.
Jeff
Robert, on my current locomotive wheel the waterlining is useless. I have the transition point set at 45 degrees and not only does the parallel finishing overlap the waterline region almost totally, the parallel now jumps back and forth over the workpiece surface instead of progressing orderly across the surface. Maybe it is because of the multiple recesses the spokes provide, but I am sticking with X-Y parallel because it works flawlessly.
Likewise the penciling is still not quite up to snuff in that I need to push the tolerance much finer on the penciling to get a reasonable toolpath vs. parallel. And even with my 3GB memory now that takes significant time…
P.S. A small thing, but the one setting that seems to still not be sticky is the MC window size itself. It always reverts to a small window the next time I start the program.
Randy
Randy,
The window size comes from the start-up short cut, right click and look at preferences, select Maximized.
I thought that you had learned about asking for little Installer changes
Jeff
Jeff,
No, window position is usually a registry entry. [where's that evil grin emoticon?] I don’t start programs maximized–I leave a strip of icons visible on the left side of the screen and toggle apps from large window to maximized as necessary. It’s not a biggie in the grand scheme of things and I can certainly live without it!
Two things I have discovered about penciling–going from .001 to .0001 tolerance does not have a major effect (on my current workpiece), and the pencil toolpath generation does not report back with a calculation time as do the parallel operations.
Randy
Randy-
Can you send me the STL of your current wheel with a description of the tool you’re using?
Daniel-
I think this is actually the correct behavior that, in a non-intuitive way, makes sense. If two flat regions are next to eachother but at different heights MeshCAM will link them together. This would cause a stairway-shaped item to be machined in one big region instead of each region being handled separately. This will be changed with the next toopath upgrade after the current one is complete.
For an analogue form like a face or something artsy, with few or no parallel flat surfaces that could be correct behavior. However for the parts I intended to machine the stairway approach is definitely not appropriate. For my part (pic in MC yahoo group) the correct approach would be a roughing operation that consists of Z-axis slices, each slice would be divided up into pockets. These pockets would be first water-lined. Then the resulting plateau would be removed via X-Y rastering or X-Y Spiraling, without the tool Z changing until that plateau is finished. Also during the plateau removal the tool would not overlap the waterline more then the step over distance which would probably be 45% of the width of the waterline pass. The finish path for this part would be a waterline again but this time it would be a finish water line, the first roughing waterline should have left a specified amount of stock. Also a pencil clean up and lastly ( very important that it be last) a parallel finish which only machines the flat remaining top and bottom surfaces and never touches the perfectly smooth waterline finished sides; it should stay the tool diameter minus the step over distance away from the water lined walls at all times. In short …flat continuous surfaces parallel to the table should be plunged into once and rapid-ed out of once. And the path of parallel should never exactly over lap the waterline it should be offset so as not to ruin the waterlines finish.
P.s. My Evaluation license expires in 14 days, do you expect to have another release before then? I would be happy to buy if I can verify the few remaining issues have been resolved.
Daniel-
I agree about the optimal behavior but it is very difficult to make a toolpath “optimal” even with clean input geometry- never mind the strange but valid files that people email to me. The goal of MeshCAM is to generate a good toolpath quickly without tool much involvement from the user. I expect this to always improve but optimal is a very tricky. It’s tough to predict the future of MeshCAM more than a month or two at a time. If you need more time to evaluate and watch the development then email me when the trial expires and I’ll send a new code to you. I would expect several releases int he next month or two.
-Robert
Just found an old bug. Retract to Z0.000 with waterline. Does not show up in cut viewer, but does when cutting parts. Easy way to check is look for Z0.000 in the .nc file. Robert, if you need more info, let me know.
-Adam
Adam,
I tried really hard but couldn’t reproduce your Z0.000 problem with 6903. It always used the ‘Set Retract Height’ (Stock Max Dist) with a simple and short test file. I was using one of my weird post files, which are you using?
More details please, I get really frustrated when I can’t find a way to repeat and document a bug.
Jeff
How to.
Here is the part file and the cut settings. You can see both the water line, and pencil cutting right through the top of the part, Z0.000, so, in my case, into my part.
http://www.batbuilds.com/~adam/new_bug/end caps small.stl
http://www.batbuilds.com/~adam/new_bug/bug_settings.JPG
Can you repeat it?
Adam,
Although there are tool passes at z=0.0000, the toolpath does not cut into the part because the part nor stock does not extend above z=0.0000
http://www.prototrains.com/misc/endcap-cutviewer.jpg
Really, this part being a vertical-sided and flat-topped prism is a job for SheetCam. It is the kind of thing that SheetCam is made for. Meshcam is really for 3D shapes (i.e. contoured.)
If the top surface of your part is important, make it .010 or so taller and face it as a last operation. I often add “safety stock” to my pieces when I absolutely positively don’t want a cutter touching a previously-machined surface. Sometimes this takes 3 or 4 versions of my solid model to “hide” and “uncover” various parts of the surface. And this is on a Tormach with preloaded ballscrews. You need to accept the fact that no machine is perfect, but CAM software assumes perfect machines. Even Mastercam.
I don’t see this as a problem with MeshCAM. I use MC and SC to complement each other–often times on the same workpiece.
Randy
OK, thank you for info. My CNC is far from perfect
Normally I am cutting complex curves, wings. That part is for the next revision of the CNC, still aiming for perfection.
-Adam
Adam, I worded that badly. I was not dissing your machine.
I should have said “No machine is perfect, but you must account for the fact that all CAM software assumes perfect machines.”
Randy
Adam,
I can reproduce your problem with Z0.0000. You are right that the retract height seems to not be working right.
Since I know that my stock is not going to be flat I always offset the top Z position of the stock. (by habit .5mm which is also my normal retract height) Sort of like Randys “safety stock” model modifications.
And Randy, both of my mills would be deeply offended by your comment about machine perfection. Both have the capability of a net connection, the only thing saving you from a barrage of hate mail is that they are too dumb to figure out email
Jeff
Jeff (and Adam),
Both waterline and pencil are using the retract height for rapid moves:
http://www.prototrains.com/misc/endcap-waterline.jpg
http://www.prototrains.com/misc/endcap-pencil.jpg
But I think that Z=0.0000 is a valid depth for the waterlining in the progression 0.0000, 0.1000, 0.2000, … , depth increments. Just to make things even harder for Robert (and yeah, I should know by now to keep my big mouth shut) maybe what is needed is a switch to allow/disallow waterlining at Z0.0000 in case the top of the part happens to be there… Forget I said that, OK?
:D
And Jeff, I was not dissing your machines. I should have said “Hardly any machines are perfect, but you must account for the fact that CAM software assumes all machines are as perfect as Jeff’s.”
Randy
Oh, and I forgot to point out that my reasoning is because the waterline moves at Z0.0000 are feed moves (yellow) rather than rapid moves (red)
Randy
Arrrrgh, a whole post of mine was deleted.
I pointed out that both waterline http://www.prototrains.com/misc/endcap-waterline.jpg and pencil http://www.prototrains.com/misc/endcap-pencil.jpg are using the retract height for rapid moves.
I further pointed out that z0.0000 seems to be a valid waterline machining depth and that maybe there might be a call for a switch to prevent waterlining at z0.0000.
I’ll leave out the silly remark about Jeff’s machines and see if this passes the moderator.
Randy
Ok- I’ve been a little mentally slow lately so it took me a while to figure out what the complaint was. I’m too close to the program and sometimes I see no problem with behavior that others report as a problem. I think I will probably eliminate any waterline at z=0. MeshCAM already assumes that there is nothing significant above the stock so it’s really a waste to allow a toolpath at the top (unless it’s a parallel pass that could act as a facing pass). Consider it added to the todo.
Tempting as it would be I won’t add to the machine dissing- I leaned long ago that pointing out to people that a Sherline or a Taig won’t hold .0001″ tolerance can be more contentious than politics or religion. Pointing out to someone with a bigger machine like a Tormach, as I now have, that a poorly programmed toolpath/feedrates, poor tool selection, poor stock material, etc. can ruin tolerance is even more futile (What do you mean I can’t machine pine to within .001″ with a 5″ long cutter at 50ipm?). All support emails that I get relating to this topic now get very a non-judgemental reply.
-Robert
I am hurt Robert! Are you stating that my CNC made from wood, plastic, and duck tape cant hold to 0.000000001!?!
All joking aside, thank you for the status update, and getting this one on the “to do” list.
-Adam
I really need to thank you guys for point this type of thing out. It really is hard to see some really obvious things after you’ve looked at them a few hundred times.
I’m sure your machine will hold that tolerance- you used those NASA 2×4’s and Northrop Grumman duct tape to make it right?
-Robert
Hey, Robert, there’s no dissing from this end! I have nothing but respect for guys like Adam and Jeff who have built up their own machines.
BTW, Adam, the quick workaround for your immediate problem is to replace the Z0.0000 with Z0.0500 or whatever in your text editor. There are only 7 places in the nc file. But you probably did that already!
Randy