Loss of detail when 3d machining

I have posted on the Vectric forum as well hoping to find some suggestions.

I have been running some 3d finishing toolpaths and the detail just is not there according to the preview from my VCarve software. I am beginning to wonder if my problem isn't coming from a setting in my Linuxcnc software or post processor that I am using.

I have a home built machine that works fine running 2d tool paths and maybe for some they would say that my 3d toolpaths are ok too, but I am looking for more detail based on the software previews.

I am wondering about my constant velocity settings. My PP is set to G64 P.005, which I would think would be more than sufficient. I have tried reading up on this and just get more confused. I understand that my 'P' tolerance is how far the tool path is allowed to deviate from the code. A couple of questions that I have are, do I need to also have a 'Q" tolerance specified and my second question is would I get sharper detail if I set G64 to P0, ultimately turning it off (as I understand it)?

My 3d toolpaths take long enough to run as it is, I don't want to compromise too much speed for lack of detail or vice versus. I am open to any suggestions.

I have included pics of the preview and of the finished part. Also including my .ini file.

Thanks

previews are just that , they do not bear resemblance to the finished item ,
base everything on the finished item , never outlines or previews . they are only a guide , and nothing more
mostly to pick up on the obvious errors , not fine detail .

I understand your opinion on previews, but the people at Vectric pride themselves in suggesting that the final result will look like the preview if the user inputs all the tooling specs correctly. I don't know if you use any of their products, but the selling point to me was the ability to preview projects before you spend the time running the actual toolpath.

That being said, I appreciate any help. I am still looking for help regarding CV settings. I just finished running another test of the loon. I changed my G64 tolerance to .01 from .005 and I also decreased my Z axis max velocity by 1/2. While my toolpath ran considerably faster, the quality in the detail was worse, if anything.

I am currently doing a test with G64 set to P0. While I know this is NOT going to be as smooth running, I wanted to see what effect it has on the detail.

To be honest I'm not sure what G64 P0 will do. G64 with no P will be the fastest possible speed while still touching every line segment. The Q term treats lines that are "Q" away from co-linear as a single line, and if unspecified is equal to the specified P. I think there is a possibility that setting P=0 may do the same thing as having no P. I would suggest just using a much smaller P (P0.001 or 0.0005). The details that I think you are complaining of loosing are extremely fine, and I think they could easily be lost with blending set to .005.

That said the media you are working with (wood) is also limited to the amount of extremely fine detail it is capable of reliably showing.

Finally, and this may be your bigest down fall. Your machine (in its current state) may not be capable of it. from the looks of the picture of your carved piece. It looks like your machine may have some backlash/stiffness problems that might make this impossible. With the detail sizes your looking for any backlash is going to be unacceptable, and backlash compensation isn't going to cut it. Also run out and looseness in your spindle bearings could easily obliterate the finer details.

and of course to add to Todd's comments , your cutting tool , type & size along with spindle speed , i doubt G64 will help to the extent that you feel .
i have a feeling we just not hit the nail , without knowing more of your machine and it's capabilities.
wood can have so many problems , with density & porous properties , that are not apparent to start with as well .

If you are concerned with what g64 is doing and want to disable it you can try g61
linuxcnc.org/docs/html/gcode/g-code.html#gcode:g61-g61.1
Also check your g code to make sure that the g64 settings are not being changed during the course of the run.

Rick G

Thank you to all who have replied.

An update on my last run with G64 P0. Results were much better with more detail, smooth transitions and no stepover marks. The run did take a little longer, but was definitely an improvement in quality making me believe that it can be done.

I am currently running the who ornament again leaving G64 set at P0, but I raised my Z axis max velocity back where I started. Hopefully that won't be an issue.

As far as the comments about my machine...they are all warranted and some of them probably true. I am using a quality tapered ballnose from Precise Bits. It's a .0313 4 flute. My router is a Bosch Colt with quite a few hours on it and I suspect the run out probably isn't good. I may have unrealistic expectations with what I have to work with...but it's what I have.

I will post a pic when this run is done...hopefully it will be better.

Thanks again!

try 2 flute bits

What would the advantage of using 2 flutes over 4?

In cutting wood you need high RPM (such as what you get from your router), With 4 flutes it will be impossible to achieve an adequate chip load to keep the bit cutting, rather than smearing and burning, prematurely dulling the tool. In fact I doubt even with a 2 flute tool you'll be able to go fast enough in small contours to maintain ideal chip loads.

In other words, for wood 1 and 2 flute bits usually work best.