[cncgg]

I used to run a Thermwood at work and it had a setting for resharpend bits. If the bit is programmed with a .5 diameter and then you resharpen the bit, it is less. We had a setting we could enter in the machine and it would adj the program.
Currently I have an LC series and use Vcarve pro as my toolpathing program and have to change the bit diameter in the software and repost to machine with the new resharpend bit size.
Does Techno have this feature? Also attached a screen shot of a setting Im not sure what it does .
Thanks, Glenn

[ger21]

Actually, this is a function of the g-code, and not necessarily the machine. If your g-code uses cutter comp, you just need to change the tool diamter in the machine's tool table. That's how the industrial machines that I've used have worked, and I assume the Thermwood is the same.

UNfortunately, V-Carve Pro doesn't support cutter comp.

[RandK]

The Techno controller doesn't support the G-codes and cutter diameter compensation. It's really nice to have.

[Dave's_Not_Here]

RandK

Aspire has a tool edit feature when tool-pathing any file. Can't you just edit the dimensions of the new cutter or copy and rename a cutter and edit it to the new size? VCarve Pro should have the same capability.

[Montabelli]

most software packages will allow you to set the cutter comp in the control or in the computer, the control capabilities are what determine if the g code can be read and the offset calculated during the run. Techno's control never had that capability, though I believe Eric was working on it when Techno went out.

[Dave's_Not_Here]

ger21,

Understood. I wasn't aware he was a high production shop, especially when he uses VCarve from Aspire. The VCarve program he specified, has a tool database (tool table) which will allow him to build many 1/2" diameter cutters and profiles. It also allows him to edit a specific cutter to a smaller diameter and assign a new tool number and name to it if he wants. He can then do a recalculation of any or all toolpaths on the fly. Takes maybe 30 seconds in most cases, for VCarve.

Even in your scenario, doesn't someone, at some point, have to enter the actual diameter of the sharpened tool into the tool database/table? I don't use cutter comp, obviously, but whether he does an auto recalculation of the toolpaths in VCarve after entering the diameter or recalculates based on cutter compensation, what difference would it make? He is still doing what you described... editing the tool database with a new diameter and recalculating toolpaths. He can assign tool numbers and names for all 15 different cutters if he wants or use cutter compensation. Regardless, someone has to enter 15 different diameters, as the software doesn't intuitively know what to compensate for. I realize my ignorance of cutter compensation is showing, so if I am way off base, please make allowances or compensation

[ger21]

Even in your scenario, doesn't someone, at some point, have to enter the actual diameter of the sharpened tool into the tool database/table? I don't use cutter comp, obviously, but whether he does an auto recalculation of the toolpaths in VCarve after entering the diameter or recalculates based on cutter compensation, what difference would it make? He is still doing what you described... editing the tool database with a new diameter and recalculating toolpaths.

No, you don't. Toolpaths are created (using cutter comp) using the full diameter of a new tool, so 0.50, 0.25, 0.375, etc.
The machine has a tool table with the actual tool size.
When the g-code is run, the machine compensates for the actual tool diameter.
If you program for a 0.50 dia tool, it doesn't matter if the tool is 0.489, or 0.437, or 0.50 with a new tool. The part will always be the correct size, using the original g-code.
That's the beauty of using cutter comp. There is no recalculating toolpaths. Toolpaths are created once, and can be run with different tool diameters with no changes needed. We cut maybe 1500-2000 4x8 sheets of melamine each year, with a 1/2" compression spiral as tool #1. 95% of those sheets are cut with a sharpened tool that's less than 0.50 diameter, but the thousands of parts are all programmed using tool #1 with a diameter of 0.50.
I can program 100 parts right now and cut them with a 1/2" tool.
If I need to cut those same 100 parts tomorrow, but only have a 3/8" tool, I just enter .375 in the machines tool table, and all 100 parts will be cut to the correct size, using the same g-code created for the 1/2" tool.

We may literally create thousands of programs a month. The tool diameters in our CAM tool table never change, and are almost always different than the actual tool diameters used to cut the parts.

Now, if you had 1000 programs created in V-Carve Pro, and wanted to use a different tool, then you'd have to load the 1000 programs back into V-Carve Pro, and recalculate. I don't have to do that.

I do use Aspire at home, btw, so I'm very familiar with what you're describing.

[Dave's_Not_Here]

Gerry,

Thanks for the info. I have a better understanding of compensation. Seems to me if Glenn has a lot of projects that require a lot of manual cutter compensation and an ever-expanding project file, than something other than VCarve to generate toolpaths would be in order, especially since Techno will not be forthcoming with any new interface upgrades.

[ericscottf]

Howdy all,

I wrote a piece of software that modifies Gcode to apply cutter compensation for resharpened bits. The main issue with it is that the G-code must reflect the "direction" of the cut (G41/G42). Basically, if you're cutting a circle, in order to compensate, the system needs to know whether you want the donut or the munchkin, as I like to say. I added a bit of functionality to make it so you can hand-edit the G-code to indicate a "universal" direction - useful if you have a file full of donuts or munchkins only. The software works with the Techno plugin system or on it's own, so it can be used with most systems that lack Cutter Compensation.

Long story short, it's very good if you have very simple geometry, but for complicated files, you're better off going back to the CAM package and re posting with a modified cutter. I wouldn't use it to change from a quarter inch cutter to a half, it's really meant for comping a few thou due to cutter wear or deflection. If the compensation would cause more than one element to need to be removed, the file must be re-posted.

If anyone is interested in it, shoot me an email and we can discuss to see if it fits what you're doing.

Eric