Post Processor Help

[paramedicpops]

Looking for some post processor help. I am using a CNC Shark HD 2.0 with Aspire 8.0. I do a lot of 3D carving and recently have had detail loss when making repeat carvings with my saved files. I look at the processors and now see what looks like a new one. CNCShark-USB 3D Contour? I have been using CNCShark-USB Arcs. Should I change to the 3D one? Thanks everyone!!

[Rando]

I took a look at mine, and it looks like the only difference is the G64 "Best Speed Path" line. In the 3D Contour one, it's 0.050", but (at least in mine) it's 0.005" in the non-contour, arcs one. That said, mine might have been modified; I tend to do that . The line appears up in the "Header" section near the top. That G64 command disables the "full stop" mode in more-standard GCode implementations. Here's a link to a halfway-decent description of that:

http://machmotion.com/cnc-info/g-code.h ... ntrol_Mode

When G61 is set, (yeah, it probably should have been an M code, but whatever) it means that the controller will come to a complete stop at the end of each block, or move segment. That deceleration and then acceleration is both hard on the machine, and makes the cuts less precise. The G64 command, turns that off so that the controller "looks ahead" to the next move, and tries to keep the XYZ motors moving smoothly. This can sometimes cause "doglegging" in paths, and even take tiny chunks out of the stock when it rises out of small (but tall) pocket and then rapid elsewhere. The P value in the G64 line defines the accuracy to which the controller will (attempt to?) keep the actual movement path in line with the programmed movement path.

Make sense? If you're losing dimensional accuracy, find that G64 number and make sure it's "small". Personally, I'd like it to be 0.00001", but that's not going to happen . 0.050" appears to be the default, but IMO that's only okay when you're doing wood carving of bridges. I'd turn it down to 0.005, or even smaller.

Give that a try; be sure to save the original Post Process somewhere. Also, in case you haven't figured it out yet, if you make a folder called My_PostP at the same level as the PostP folder, you can put in there (My_) the post processor files you want to see, and the Vectric software will only show those, so you won't have to search through a long list of processors you'll never use.

Hope that helps,

Regards,

Thom Randolph

[sharkcutup]

Also, in case you haven't figured it out yet, if you make a folder called My_PostP at the same level as the PostP folder, you can put in there (My_) the post processor files you want to see, and the Vectric software will only show those, so you won't have to search through a long list of processors you'll never use.

In regards to the "My_PostP", after you get it setup the way you want. it might be a good idea to save a backup copy of it in another place on your hard drive should you ever have to re-install the V-Carve or Aspire program again. If you don not do this the re-install completely eliminates it and you are back to square one!!!

As with the "My_Post" as said above in the quote can be done also for the "tools.tool.db file" in ToolDatabase. I also make a backup copy of it too!!! I have already lost my tools once it is not going to happen again. It is also a good idea to periodically save the tools database file for it changes (adding/removing/bit details) much more often than the mypost processor files.

Just a Thought GUYS!

Have a GREAT DAY!!!

Be SAFE around those AWESOME machines!!!