PDA

View Full Version : Error cutting on a z level pass



mspaw
07-12-2011, 11:50 AM
Hi-

I'm new to madcam but have been enjoying it for the most part. Im currently doing some test cuts for a plaque in acrylic and playing with different strategies for the finishing. Ive run into a couple of issues that may well be user error but at this point im not sure.

1. I'm seeing some witness marks in the profile of the pice that appear where I gather the tool is transitioning to a different area. This has only been with the z level finishing. The rest of the profile is untouched but where the tool makes this transition its been digging a bit into the work. Please see the attached image to see what the path is causing the issue.

http://morphographic.com/CNC/CNC_SpinnerLogo_CuttingError_01.jpg

2. Secondly, and ill have to dig up a screen cap that shows this. When doing a planar pass ive seen several occasions where the path will jump to a completely different are of the work piece and skip a large section only to come back to it later in the cut. This wouldn't be an issue except im seeing a trace of where the transition/jump occurred in the surface finish. Its subtle but there is a variance in the z height at the transition point. The continuously cut areas are uniform so it only seems to happen where these jumps occur.

I'm happy to hand over the file if that helps but don't want it to be public.

Thanks!

-Michael

svenakela
07-12-2011, 03:34 PM
I'll send you a PM with my e-mail adress, send the file to me and I'll have look at it.

mspaw
07-12-2011, 08:30 PM
Ive sent you a PM with a link. Let me know what you think.

Thanks!

-michael

svenakela
07-13-2011, 02:34 PM
I noticed that the Z-level path was last in your file. It should be processed before any Planar finishing.

Sometimes a model without a bottom surface can make some problem for the logic that calculates the path, but it doesn't seems to be the case with your model. I regenerated the Z-level with a 1.5 mm ball-nose and default settings and the path is perfect. I also changed the settings a couple of times and went with different mills to see if I could recreate the behaviour. But I can't.
Another thing that differs is that my path is going all the way down to the bottom of the model.

* What are your Rhino settings? Did you setup Rhino as written in the MadCAM help?
* What MadCAM version do you run, 4.1 or 4.2?
* Could you give me a hint what settings you used for the Z-Level?

The attached image is my first test with default settings and a 1.5 mm ball.

mspaw
07-15-2011, 02:15 PM
Im currently using the most current version of madcam, im on the last days of my trial , but should recieve a lic here in the next day or so.

Interestingly enough I recalculated with the defaults and the odd pathing went away. I guess it was a fluke but Ill certainly look for it the next time I use zlevel.

Also thanks for the order change that mad a difference in the final appearance.

One thing id love to know as there isnt much info in the docs or here on the forum is when to use remaching or pencil tracing. being new to cnc Im not familiar with the best practices and would love to here how people are using these strategies. For instance in the corners of my piece Id like to hit them with a 1mm ball to follow the 1/16 ball used for finishing. What would be the best strategy?

Thanks!

-Michael

svenakela
07-15-2011, 05:16 PM
You're right, the help files are pretty technical and you might need knowledge to come through a good strategy.
You could always start with checking the vid's at madCAM CAM plug-in for Rhino3D (http://www.madcamcnc.com/Support.html) and MADCAMCNC (http://madcamcnc.blogspot.com) (there are plenty more vid's coming, I know that... :))

The "standard" strategy is

Roughing - Cut down material with a big cutter
Z-level - Cutting down to edges and profiles with a smaller ball/radius cutter
Planar - Finishing surfaces with a ball/radius
Pencil trace - All mills with a radius will leave material in corners, think of pencil tracing as the last step where you use a sharp tool to get rid of that last unwanted material without running over the entire work piece once again.


There's also Remachining (depending on license level) and you use that if you want to run another roughing path for example with a new tool without running over the entire workpiece once again. It uses the earlier processed tool paths to find areas where there is material left.
Not everyone see the potential in this feature, for example if you're making moulds in steel you cut the runtime a lot for the smaller tools if as much material as possible is taken away. Therefore it's better to run another path with a smaller roughing tool before the fine paths are executed.

I'm cutting a lot in soft materials and very often I go directly from Roughing to Planar. It all depends where I save time. :)