Some CNC work....

[Doug Rasmussen]

This is a tapered spiral with a twist, not a straight taper. The flute radius varies down the taper (not done with a pattern router bit).

Hand coded and run on a M400 Centroid control using the macro language. Relatively short program with the cutter path calculated on the fly, less than 50 lines of Gcode. Blank was held in the 4th axis, sharp vee tip wheel cutter cutting on the side of the blank (as opposed to on the top).

[Doug Rasmussen]

Pyrography.

Again 4th axis on the round parts.

The burning is done either with a soldering iron mounted on my machine's quill or with a 3 watt diode laser likewise mounted. The laser is more forgiving on "depth" of cut, but diode lasers are dangerous. I've found conventional wood burning tools, even the high end variety, don't work well in this application. They get very hot and also cool very quickly when they're fed into the work leaving an initial dark impression which tapers off due to the tips cooling. My digital soldering iron maintains constant tip temperature, only 850 degrees F though which means slow feed rate.

Note the ukibori on the second to right piece's lower end.

[Doug Rasmussen]

Unicorns..?

These are done with the part standing upright. A wheel cutter moves downward in the arc paths. Then the part is rotates one degree or so and the cut is repeated dropping the starting point in Z down 1/360th of the pitch.

A very short program, again programmed in Centroid macro language.

[Doug Rasmussen]

Spiral with variable pitch, 8 flutes. Part is held in the 4th axis.

[Doug Rasmussen]

Domed end on work.

[Doug Rasmussen]

Some metal work. An alunimum die to press a flower design in copper sheet. Work piece is flat on table.

[Bruce Page]

Very impressive Doug. Are you G coding all of this by hand?
What kind of cnc are you running?

[Doug Rasmussen]

Very impressive Doug. Are you G coding all of this by hand?
What kind of cnc are you running?

Thank you Bruce.

Yes it is mostly hand coded. There might be a small segment of CAM code. For instance, the spiral pieces. there would be a few lines of code to generate the arc for a single flute. then you repeat that say 6 times around the workpiece for a six flute spiral. then you step lengthwise down the blank using the control's scale function to resize the flute giving a taper. Basically, you take a simple cut, repeat, scale it, repeat and so on and so on.

My control is a Centroid, a fairly powerful control that allows you to do things in Gcode that sometimes are easier to program than to draw. The machine is a basic knee mill with 4th axis. It's a bit larger than a Bridgeport.

As a simple example. With a basic arc command, G02, you could route a circle. Then you could tell the control to repeat the circle but at 80% of original size. Keep repeating the circle at less size and you would end up with a series of concentric circles only having programmed one circle.

[William Adams]

Way, way cool.

For anyone using the limited G-code set which Grbl supports, there’s now a pre-processor which extends that to support most of what LinuxCNC supports: https://github.com/NRSoft/GSharp — looking forward to seeing it built into every G-code sender.

[Mark Bolton]

Did you CNC the Ukibori or is it conventional?

+1, nice work

[Mike Heidrick]

I too have centroid with a 4th axis - mine is on a knee mill I retrofitted with an allinonedc. Would you post the gcode so I could see it and try and understand it. I am new to the 4th axis setup on mine. miek at thewoodworker dot net is my hiom eemail if it is easier just to email it.

Very awesome work.

[Doug Rasmussen]

Did you CNC the Ukibori or is it conventional?

+1, nice work

Yes, it was done with the CNC. A small diameter jewelers dapping punch was used as the tool. The dapping punch was held in a collet like a router bit to make the impression in the work. A skim cut with a router bit was done, then steaming to raise the pattern.

[Doug Rasmussen]

I too have centroid with a 4th axis - mine is on a knee mill I retrofitted with an allinonedc. Would you post the gcode so I could see it and try and understand it. I am new to the 4th axis setup on mine. miek at thewoodworker dot net is my hiom eemail if it is easier just to email it.

Very awesome work.

IMO, the most complicated part of 4th axis work is calculation of a rotary feed rate equivalent to the feed rate used in normal 3 axis work where the feed is expressed in inches per minute, ipm. When the 4th axis is used the feed rate has to be specified in degrees per minute.

G01 X5 F20. This would be the way a non-rotary move might written. Feed at 20 IPM from the current position to X5.

G01 A300 F1146. This is a rotary feed rate of 1146 degrees per minute on a 2" diameter piece equivalent to a non-rotary feed of 20 ipm. The feed rate is dependent on the work diameter.

Let's do the math. 2" diameter has circumference of 6.28" At 20 ipm, 20/6.28=3.18 revolutions per minute. Multiply that by 360, and you get an equivalent rotary feed rate of 1146 degrees per minute.

Anytime there's rotary axis feed it has to be in degrees per minute. But, there are controls that do the calculation internally so no need for the math. Unfortunately Centroid is not one of those controls.

Things get worse when you have a combination of linear and rotary feeds like G01 X5 A300 F1000

Here's a link to a formula to calculate combined feeds.
(http://www.cncsnw.com/4thHowTo.htm)http://www.cncsnw.com/4thHowTo.htm




(http://www.cncsnw.com/4thHowTo.htm)

[Doug Rasmussen]

In my previous post about calculating rotary feed rates I left off with no easy solution to what can be complicated.

I use Millwrite software to do the calculations. That makes it easy, Millwrite uses the flat pattern Gcode and wraps around the work of the diameter you specify.

Cncsnw also offers a program to calculate the rotary feed rates.

I have a spreadsheet setup to do it. It needs some work though, not quite ready for public consumption as it's a little cumbersome to format the
Gcode for spreadsheet input.


For a few years I've been trying to get some straight answers from Vectric whether their software will automatically calculate rotary feed rates. I had a few exchanges with Vectric tech support ending in them basically telling me I didn't know anything about CNC's. Recently an individual at Rockler told me the Vectric software had now been modified to calculate rotary feed rates, but apparently I've been put on Vectric's ignore list because they don't respond any more. Maybe someone on this forum can tell us how Vectric handles rotary feed rates currently.

[Gerry Grzadzinski]

Maybe someone on this forum can tell us how Vectric handles rotary feed rates currently.


The simple answer, is that they don't. At least not in the the program itself.

For some machines, they have the post processor output lines of code that calculate the feedrate. The post processor has access to the "wrap diameter" info, and by using that and the feedrate, they output a formula that calculates the feedrate for a axis moves.
I've never used this, and just took a quick look at the included shopbot and camaster posts that do this.

[Gary Campbell]

Gerry is correct. Vectric products do not have a variable output for rotary feedrates. That said, a rotary surface feedrate can easily be added to any controller that can accept a couple math operands. The syntax for the math line is totally dependent on what is accepted by the control software. This is evident if you look at the differences between the ShopBot Indexer and CAMaster Recoil postP's.

The formula is 360 / pi * [XY Feedrate] / Diameter or as a simple line using Vectric variables: "115 * [FC] / [WRAP_DIA]"

This is a much more appropriate feed application than some methods that actually will increase rotary feedrates as Z depth increases. Very useful in metal lathe turning, not so much for rotary wood machining.

[Doug Rasmussen]

Gerry is correct. Vectric products do not have a variable output for rotary feedrates. That said, a rotary surface feedrate can easily be added to any controller that can accept a couple math operands. The syntax for the math line is totally dependent on what is accepted by the control software. This is evident if you look at the differences between the ShopBot Indexer and CAMaster Recoil postP's.

The formula is 360 / pi * [XY Feedrate] / Diameter or as a simple line using Vectric variables: "115 * [FC] / [WRAP_DIA]"

This is a much more appropriate feed application than some methods that actually will increase rotary feedrates as Z depth increases. Very useful in metal lathe turning, not so much for rotary wood machining.

Gary, if you have a situation where a cut consists of a combination of linear and rotary motion and the linear is much longer than the rotary motion you'll be in serious trouble, metal or wood cutting. For my uses in pyrography the amount of burn (width of line) is directly related to the speed of the burner. Likewise, with tiny, fragile router bits the risk of breakage is substantial unless the feed is corrected to account for linear + rotary motion.

This business about Vectric outputting variables is news to me. Can it operate as a stand alone program producing fairly generic Gcode that would run on my machines without post processing? Typically in CAD/CAM software (which Vectric is..?) the software developer provides a wide range of post processors included with the software. As an example, Autodesk Fusion 360 includes more than a hundred post processors covering a wide range of CNC machine controllers. It appears with Vectric the machine makers may be providing the post processors, am I right?

I've attended a couple of the CNC enthusiasts meeting at local woodworking stores. More often than not in talking with group members I've had the feeling we weren't talking the same language, now I'm beginning to see why.

[Gary Campbell]

Doug...
First let me say that I love your hand coded projects. And let me add that little or nothing that I say relates to metal cutting / turning, as I have no experience in that arena.

When you say: "if you have a situation where a cut consists of a combination of linear and rotary motion and the linear is much longer than the rotary motion you'll be in serious trouble", I either misunderstand the statement or disagree wholeheartedly. For 4th axis rotary wood machining of 2, 2.5 and 3D toolpaths, setting a rotary feedrate that offers the same surface feed in the radial as axial is exactly what most users would wish for. This allows us, the user, to set feedrates that we would normally use for flat work and apply the same to rotation. A rotary axis works just like a moving table that moves material, rather than the cutting head.

All of the output from CAM software, as I understand it, is in the form of variables. A post processor is REQUIRED to ensure that the output is proper for the intended machine. So no, it would not work without one. There are numerous versions included, I stopped counting somewhere north of 400 and did not open a few folders. I believe Vectric works with OEM's to develop posts that are appropriate for their various models. The OEM's provide the fine tuning based on the features they wish to use and support.

I hope this helps

[Gerry Grzadzinski]

Vectric's software outputs g-code basically the same way that Fusion 360 does. You choose the appropriate post processor, and export the g-code.
The post processor defines the format of the g-code.
I just checked, and the latest install of Aspire has 432 post processors, plus a few additional folders with additional posts.
And yes, there's a generic g-code post included in there.

[Doug Rasmussen]

Gary & Gerry, thanks for the clarification on Vectric's post processors (strange that Vectric support didn't tell me this in the email exchanges we had).

Googling, I wasn't able to find a listing of their supplied post processors. Is there one for Centroid controls?

Thanks again.

[Jerome Stanek]

If you download the trial version you can see the posts that they have and you can learn the software.

[Gary Campbell]

There are 2 posts Centroid named. With arc support, one for inch and 1 metric

[Ted Reischl]

I use Mach 3 for controlling my machine with rotary. As Gerry stated, Vectric does not calc the feedrates. There is no need, the calcs are built into Mach 3. Sort of fun to watch the machine speed up as the diameter decreases.