Can PhotoVcarve be used to Laser engrave on a CNC Router????

[Ms Wolffie]

What a great source.
Thank you, I have bookmarked it.
Cheers
Wolffie

[JJWMACHINECO]

Here is another one I did with my Laser from that web site. I spent aome time focusing my laser a little better and I'm very pleased with the results.

[JJWMACHINECO]

Here is another one I did today.

[JJWMACHINECO]

Decided to scan one of my antique glass negatives today and lasered the image. Used Line Art this time instead of Jarvis to convert to black and white.

[dlgabry]

Looks great Jeff! I have a lot of trouble seeing exactly where the focal point is. How did you go about finding it?
I'm staying with the setup I have, with the Z direction line controlling the laser. It's way faster than the analog photointerrupter I was using. Since the Z stepper isn't being used, I can boost the acceleration rate for Z way beyond the stall point for a stepper motor.
I've been playing with halftone images with promising results, though the halftone programs as well as pvc have presented some issues. It seems that the halftone dots for the darker areas actually touch, and pvc turns that into one long move to traverse the dark area, which in turn allow X and Y to reach full speed giving the dark areas a washed out look. I'm testing with Jason Dorie's halftoner tool, it allows you to specify a min and max dot size and also lets you specify the dot spacing. Unfortunately, it doesn't save a shaded bit map image, but it does allow saving a dxf file which can then be manipulated into a shaded bitmap for PVC.
In PCV, there's another minor problem matching the tool path line spacing with the halftone dots as the distance between lines display value is rounded off to 3 decimal places, so when it says 0.005, it really could be anything from 0.0045 to 0.0055. Doesn't sound like much, but it eventually gets out of step with the center line of the halftone dot pattern and leaves an odd looking striped pattern.

This laser can also do some really small text engraving running. Made some for my better half to hold in her hand while going through radiation therapy. Turns out that many of those that she met also wanted one too. It's been said that there are no atheists in foxholes, I think oncology wards can be added to that list.

Dave

[JJWMACHINECO]

First I want to say, our thoughts and prayers go out to your family.

Dave, those came out fantastic. I was able to focus my laser by using a black anodized piece of aluminum. Anything black will work as long it does not burn while you are adjusting it. Black does not reflect the beam so you can see when the focal point is the smallest and roundest. First you need to get the right focusing of the lens in your laser, then the right distance off your material. To make your code output to a 4 decimal place. Read this about editing post processors and download the PDF file. http://www.vectric.com/forum/viewtopic.php?f=4&t=6213

I tried Jason Dorie's halftoner software and it made way to big g-code files. I know you have heard this before many times, but you get what you pay for. Even though the software is a free download, it may not be the best software to use in some cases. I'm very happy with the Corel PhotoPaint software on how it processes the image before bringing into PVC. It has halftoner also, but I did not get very good results using it. Some images, like the Trolley, I used the Emboss function before converting it to black and white. It seems to bring out more detail that way. I have learned you have to take each photo/image one at a time on how it needs to be processed.

Also I found out the washed out look was from the feedrate exceeding what the power of the laser could effectively burn the wood at. 40 IPM is max with my laser. Since yours has more power, you might be able to run at 50 IPM, but what type of wood your using will determine that also.

Jeff

[dlgabry]

Jeff, thank you!
I'll have to play with the focus some more when I get a chance.
That halftoner does indeed make some really big gcode files. They appear to be a drilling tool path using a vee bit to a depth to cover each halftone dot. They run slow on my machine. I found that I could save the image as a dxf of all the halftone dots, import that into turbocad and paint them all black and save as a bit map, then import that into pvc.
The stepover issue I had in pvc was due to its distance between lines being rounded off to 3 decimal places. For example, say the dots are .025 on centers, and range between .020 and .007 in diameter. I set the stepover in PVC so it read .005, but the gcode it produces may have a stepover ranging from .0045 to .0054. If it's not some sub multiple of the actual distance between dot centers, it eventually gets out of step with the dots. I got around that by noting the percentage where it just begins to read .005, the percentage where it just turns to .006, and setting the actual percentage halfway between. If pvc showed the real value for stepover, it'd make life easier, but I realize that we're not using it for its intended purpose. The nice thing about the halftoner output is that the dots don't actually touch, so each is done separately - no more washed out areas. It'd be real nice if it saved a halftoned bitmap

I tried a run last night at 65 ipm @ 70% power that didn't come out too bad. Maybe playing with the focus will help the clarity. Actual speed according to mach3 varied between mid 40's to low 60's ipm-wise based on the dot density.

Dave

[JJWMACHINECO]

Sorry Dave, I guess I misunderstood what you were talking about as far as the decimal place. I get what your shooting for now with the halftone images. Shades created by the size of the dots. Maybe you should try creating the code in DotG.

[dlgabry]

No problem Jeff. Yes, that's exactly what I was trying for, simulating a shaded image by hitting just the dots.
As you point out, there's a difference in the wood used too, I had pretty good luck with the 3mm birch ply from Michaels if used without doing anything to it. However, after sanding off the burn to make another try, it's real hard to burn.
I picked up some luan ply and found that it burns really really easy. Thought I remembered that luan ply was sort of whitish with little grain, but this piece is sort of reddish with grain. Cheaper than birch ply too!
Tried downloading dotg, my AV software flagged it as containing a virus and deleted it.
Did some more digging in pvc, found that although the bitmap has round dots, pvc shows the image with dots that are no longer round. That may be part of the problem with hitting the dots too. From all that I've tried though, PVC still wins the prize for the smallest gcode files and speed.
Dave

[JJWMACHINECO]

From all that I've tried though, PVC still wins the prize for the smallest gcode files and speed.
Dave

I totally agree.

[dlgabry]

Finally getting consistently good results with the laser after much hair pulling......
I'm using the z direction line to control the laser instead of the z stepper motor, with the laser being on for z- moves and off for z+ moves. That allows the z acceleration and speed to be set way higher than what would stall a stepper motor. I cut in the Y direction, and have Y accel and speed set just below the missing steps/stall setting. The z depth settings in PVC are set to get just 0.0003" above and below zero (one step each way for my machine).
Managed to avoid stepover line-up problems with halftone dots by using lines instead of dots. The halftone dots or lines touch each other in black areas of the image, which can lead to washed out dark areas if the feed rate is too high. Fixed that by brightening the darked areas so there's no truly black areas before halftoning. Gcode-wise, the halftone dots/lines result in separate plunges/retracts, which slows the feed in areas to be burned, but allows the specified feed rate to be reached on areas to be skipped.
The blurry result I was seeing (looked much like backlash in Y) was actually due to Mach's CV. Used a CV distance tolerance setting of .010 along with plasma mode, problem gone. Probably can use a larger setting with larger pictures.
Result of all this is that I can use a high feed rate without worrying as much about the speed being too high in areas to be burned. Attached pix is about 6" x 5.5", was done at 75 IPM, 25% power on luan ply, which burns incredibly easily (at least this particular piece). Took about 1 hour 45 min.

Dave

[JJWMACHINECO]

That looks real good Dave. Was you able to focus the beam down any smaller? If your only running at 25%, it looks like it's burning pretty good. Have you tried it at full power yet and how did you end up controlling the power level? Are you putting 1.25V to the modulation to get your 25% power? What voltage is the direction line you are using and how are you regulating the voltage?

[dlgabry]

Hi Jeff,
Yes, 1.25V should be 25% power if they're right about the linearity, they said 0V is 0%, 5V is 100%. Right now, I have the Z outputs from Mach going to pins 14 (direction) and 16 (step) instead of configuring them to the pins the stepper driver board expects for Z. Pin 14 drives the photo-emitter in the optocoupler, and the phototransistor output triggers the laser through a 10K pot so I can set the power level. I need to boost the power to 60-80% to burn on the birch ply from Michaels but the luan burns so easily I'm almost afraid to leave it out in the sun
It's easy to set the power level with the laser key switch off, just jog down with a meter on the line to the laser and adjust the pot to the desired voltage, jog back up and the voltage goes back to zero, turn the key on and hit the go button in mach3. I'm using a z 'movement' of one step up or down from zero - of course, the z motor doesn't move. I configured the A-axis in mach so it runs the Z-motor to make it easier to change the laser to target distance.

Pin 14 is pulled up to the 5V from an external regulated supply, pix attached. I have the direction line to pin 14 configured as active low in Mach. In the pix I attached, all the +5 and Gnd lines hook to the external supply's 5V and Gnd lines, and the external supply's gnd line is tied to the parallel port's gnd pines (18-25).

The direction line from the parallel port output pin should be either 0 or +5 depending on the direction last used. Some pc's, notably laptops, seem to use 0 and 3v on the parallel port output lines.

I'll still have to burn at a slower speed for real black and white (non-halftoned) stuff to avoid the washed out black areas I think, still playing with that. I want to try some images from the clipart site you found.

Dave

[dlgabry]

Looks great Peter!
I'm assuming that your custom post processor changes just the VAR Z_POSITION and VAR Z_HOME_POSITION so that it uses the letter C in place of Z to create the g-code?
Dave

[P.Passuello]

Looks great Peter!
I'm assuming that your custom post processor changes just the VAR Z_POSITION and VAR Z_HOME_POSITION so that it uses the letter C in place of Z to create the g-code?
Dave

That's about the size of it.
As you saw I still need the Z to work properly to focus the laser onto the stock but once that is done I don't need it again.
I decided the best idea was to set up a laser post processor and that way I don't need any special profile in Mach3.

If it is of use to anyone here are the VCarvepro and PhotoVCarve Post Processor files I made for the LaserShoe.
I have not tested the PhotoVCarve one yet and they are only for metric.

Cheers
Peter