[MecAut]

Hi guys,
I have been experimenting a bit with halftone images (great challenge by the way). My friend asked me to make something nice with his favourite daughter's photo.

The issue is, my CAM software shows an uniform simulation result without any problems, however the milled part has some VERY weird dots.

Milled part, please note the non uniform dots - no idea what happened
Attachment 316780
*please note that I have interrupted the milling as I noticed the weird pattern.

This is the original CAM simulation screen, I can't see anything wrong with the dots
Attachment 316782

My assumptions at this moment:
1) Artcam saved the relief in .tap with wrong code (some random crap)
2) My Mach3 has a configuration problem - and I don't have any clue what could be causing this issue.

Is there any software to help me debugging the gcode visually? I mean I'd like to be able to read the .tap file and manually find each .tap line represents the wrong circules. That could help me confirming if was Artcam or Mach3 error as I can confirm if the .tap file is really spot on or not!

Tis!

[Dan911]

I came across this free program and got some great results. You can also export it as a dxf and import into your cam software.

Halftoner

CNC Software

[MecAut]

I came across this free program and got some great results. You can also export it as a dxf and import into your cam software.

Halftoner

CNC Software

Hi Dan911,

I used exactly this software to create the dxf file and this software is great. The dxf is perfect, the circles (or dots) have correct sizing both on my CAM software and Corel/Illustrator.

The problem is after creating the relief there is a mismatch between what the CAM software showed on its simulation (its perfect) and what was really milled.

Missing motor steps are not likely to be the problem as my machine runs servos.

[victorofga]

try to localixe on the ready part the bad spots

or just one.. select that one spot with surrounding dots
and that 15-20 dots make a toolpathing..


if it cuts circles then the possible issue, some circles are calculated outside
and bad spots calculated inside..


but this way very hard to give any opinion because you didn't give enough detail..

can you post some of the dxf file?

select an area and save that separated area so we might have more insight..
make sure the snippet of the dxf contains the ""darkest"" and "lightest" area

[victorofga]

also if you can post the g-code, or at least the 30-40 percent of I can open editor..

[Dan911]

How many lines of Gcode? Mach 3 gets the hip cups with large files and display on. Like Victorofga says, would need to post dxf file/gcode to help analyze where the problem is,

[MecAut]

How many lines of Gcode? Mach 3 gets the hip cups with large files and display on. Like Victorofga says, would need to post dxf file/gcode to help analyze where the problem is,

I had to split my artwork in two as my old laptop was struggling. I have tried to mill just the first half. The first Gcode file had 32517 lines ...

Attached, please check the .tap file and the .dxf, both zipped.

Please note that I did not finish the whole milling process, when I saw the wrong dots I cancelled the job.
Attachment 316964

The top bit I have milled, The red box represents the detail view, matching the detail view on my CAM software (next images).
Attachment 316966

CAM Simulation
Attachment 316968

CAM Simulation detail, no non-uniform circle or any really crazy dot....
Attachment 316970

Thanks in advance

[Dan911]

Theres only 32,519 lines of gcode so I don't think this is a large file issue with mach. It took a couple of hundred thousand lines before I was able to see a problem, and just shutting off my display in Mach fixed it.

Just with a quick look at your dxf file, there was almost three hundred open vectors. Did you close these vectors before exporting to a .tap file? What cam software you using? I spent little time messing with the Halftoner program but seen it exported messy dxf vectors and needed cleaning up, I think you would be better off exporting a gode file from there unless you are able to clean up in your cad cam program. Will take a closer look at gcode tonight.

Dan

[victorofga]

if theres open vectors, then that explain all

with open vectors the program randomly will calculate ""inside-outside""

the random here means how the program interpret the direction of the vector..

[victorofga]

as you calculated a vcarving toolpath it made outside a circle.. while closed vectors were made inside

go back to artcam, and within import dxf select automatically close vectors

or, after import in the vector rolldown menu close vectors.. and all issue will be fixed


inside didn't made circle inside likely a drilling toolpath due its a circle


so for your question to finding, choose all G2 and G3 code line

they are the bad spots


edit

later back and show screenshot

the spots on your picture about parts they are looking same position then open vectors

however the toolpath shows same depth and no error..

on the upper left corner, in the second row under the sixth on right a ""bad"" spot... but toolpath shows right..
however your stuff isn't.. what you milled..


later back afternoon..
right now I have to go..

[MecAut]

Theres only 32,519 lines of gcode so I don't think this is a large file issue with mach. It took a couple of hundred thousand lines before I was able to see a problem, and just shutting off my display in Mach fixed it.

Just with a quick look at your dxf file, there was almost three hundred open vectors. Did you close these vectors before exporting to a .tap file? What cam software you using? I spent little time messing with the Halftoner program but seen it exported messy dxf vectors and needed cleaning up, I think you would be better off exporting a gode file from there unless you are able to clean up in your cad cam program. Will take a closer look at gcode tonight.

Dan

Yes, I did close the vectors in Artcam before creating the .tap. Actually without this step I could no even generate the v-carve operation.

Maybe even closing the vectors the vector quality still crap...I don't know really

Thanks

[cyclestart]

Why are there G02's and G03's in a toolpath that can be defined by plunging a v-bit ?
The only thing that comes to mind is a depth limitation applied in the software settings.
I've used the Halftoner program and used it to create the gcode. No problems.

[Dan911]

The problem is when exporting to DXF from Halftoner the circles are converting to splines.

[MecAut]

Why are there G02's and G03's in a toolpath that can be defined by plunging a v-bit ?
The only thing that comes to mind is a depth limitation applied in the software settings.
I've used the Halftoner program and used it to create the gcode. No problems.

No idea.
The workflow using Artcam is pretty simple:
- I have imported the dxf file
- Clean/fixed the bad vectors using their cleaning tool
- Created the v-carve relief, letting Artcam to define the maximum cut depth for each vector based on my tool parameters (v-bit, 60deg). That was a shallow cut as the circles were not big...

[victorofga]

no it is not artcam neither the dxf
it is only your machine

the toolpathpreview ok,

the dxf practically ok

the G code is ok

this halftoner program for others work

only you had bad result..

the picture shows the identical toolpath, what was on your cut bad, the toolpath is ok...

error happen only at your machine..

[MecAut]

no it is not artcam neither the dxf
it is only your machine

the toolpathpreview ok,

the dxf practically ok

the G code is ok

this halftoner program for others work

only you had bad result..

the picture shows the identical toolpath, what was on your cut bad, the toolpath is ok...

error happen only at your machine..

Great.

The second part of the challenge is trying to find out what happened.
- Cutting tool not properly fixed - not an option as the job had successful dots after the bad ones.
- Missing steps? I believe my servos should flag that - I'm not very good on servos to develop this subject more
- My Mach3 + Old computer had a hiccup (?)

I will try to run this again (at least the first lines)....

[Dan911]

You can easily shut the toolpath screen in Mach3 to test and run the gcode to eliminate that being the possible problem. Since the program/gcode continued to run correctly after error its not likely its a mechanical issue IMO. I wouldn't be so quick to rule out its a software cam issue. I would of liked to have tried to run the gcode like Victorofga but it was written with a metric pp and I'm set up imperial. I did load the DXF into Artcam following your work flow and yielded poor results.

1. I imported dxf with "Automatically rejoin Vectors " checked.
2. I used " Join Coincident noids" told me 6500 closed 0 open vectors.
3. Used Vector doctor and didn't reveal any open vectors.
4. Calculated toolpath with v-bit carving.

You can see in picture the messy toolpaths its making for circles(splines). Also notice the circles with no toolpaths that were ignored because were open vectors(no warnings when calculated0. The picture only shows 2 but there was easily over 100. I think different systems can produce different results when dealing with open vectors. I also MUST add the simulation showed perfect.

Attachment 317176

By using this workflow with changing splines to arch's I think may fix your errors, but know for sure it will Drastically reduce your cutting time with smother and cleaner cuts.

1. I imported dxf with "Automatically rejoin Vectors " checked.
2. "Fit arcs to vectors tool" this changes splines to arcs.
3, Use "close vectors by moving ends" will close all open vectors.

Attachment 317178

Hope this helps
Dan

[MecAut]

Thanks Dan, for your detailed reply.I'll carefully study your workflow.

One last question (sorry if I missed that), from my understanding I should see only plunges while milling these circles. Am I correct?

The cutter (60deg, 20mm diameter with 6mm shank) is much bigger than these bloody circles and the cutter needs to plunge only let's say 2 to 3mm. And this can be done in one single movement.

Looking at your pictures, I noticed a circular path within the circles - I did not quite understand that.

Thanks guys.

[victorofga]

yes... youre correct

the vcarving toolpath will make only a ""plunge"" unless the program sensing ""ovality""

again, the gcode you posted is correct..

that's why your simulation was ok..

after carefully checking, your errors not exactly matched with the open circles.. so open circle theory not true..


best would be go to artcam forum, and there are more folks willing to help you..

[Dan911]

yes... youre correct

the vcarving toolpath will make only a ""plunge"" unless the program sensing ""ovality""

again, the gcode you posted is correct..

that's why your simulation was ok..

after carefully checking, your errors not exactly matched with the open circles.. so open circle theory not true..


best would be go to artcam forum, and there are more folks willing to help you..

Victorofga, my intention of last post wasn't a lesson in Artcam, but was trying to help narrow down what's causing his problem he originally posted here for. A quick google search will show that a lot of controllers will ignore or have trouble with splines/beziers. That's why most Cam softwares provide a tool to convert them. This is the type of vectors you get exporting dxf from Halftoner. Thought this could be a possible cause and gave and option to check.

The Dxf he uploaded had 293 open vectors and thought possibly he missed 1. That would certainly cause the problem he originally posted for. I gave a workflow to ensure all vectors are closed.

The Mach3 large file syndrome could cause a problem like this and gave a way to check, shut the toolpath display off. A remedy I just learnt after many days of trouble shooting.

If any of these suggestion to check don't help MecAut, it may help others with similar problem. I know it was threads like this that help me trouble shoot 90% of mine.

Attachment 317334