Vectric Customer

I put a 2.5W laser on the machine quite some time ago, it has come in very handy for layout work and marquetry.

The other day I was trying to cut some smaller "coins" and was just not satisfied with how they were turning out. Difficult to see what they were and any detail. I was using a .031 dia tapered ball nose. No matter what I did, just not all that good. Then it hit me, why not try outlining those details with the laser? Here are two examples:
This is what one of them looks like before laser outlining:
These are two inches in diameter. It makes a huge difference. The total depth of these models is about .125 on a dished shape. Before outlining the dragon had no eyes or nose, same with the dolphins.

The process was pretty simple once I had the machine set up properly. The picture below shows the laser unit mounted on the Z axis:

I took some time and got the offset figured out very accurately. The easiest way to work with a setup like this is to use "workpiece offsets" in the machine controller. They are usually G54, etc. That makes it easy to switch between zeroes by just clicking a button. A shout out to Ger21 and his Screenset 2010, he designed it so that it makes it really easy to use those workpiece offsets. Best darn $20 I ever spent!

I use Corel X7 to add the vectors for laser etching. But Aspire will also do it. It is just that I am very used to Corel having used it since version 1.0.

These small lasers have very long focal lengths, mine is about 6 inches. What that means is setting heights is not at all fussy. I set up a laser post that does not output any Z motion at all. With the long focal length a difference in height of .125 makes no difference in results. I also assigned G59 (workpiece offset) to the laser so I do not have to mess with it.

What I have been doing is cutting the model leaving about .003 on it. Then I laser it. Then I recut it to final height. The reason is that the laser darkens the area around the laser cut line a bit. The cut is quite a bit deeper than .003 so the second cut cleans it up nice. BTW, I sort of goofed up on the dolphins. I changed my Y zero on the cutting but forgot to change the Y zero for the laser. A total of .015. So it is not as good as the Dragon. Live and learn -or- another case of old guy syndrome.

Smoke collection: That shoe is hooked to the dust collector. Mine has a pleated cartridge. Interestingly it sucks up the smoke and filters it right out. I cannot smell any wood burning in the shop and I have a very small shop, about 14 X 28. Evidently the dust cake catches all the smoke. I built the shoe mostly to shield the beam because it is not good for the eyes at all. It just slips over the Kent dust shoe mounting plate. I may get around to building a magnetic one.

Originally I started out wanting to cut "coins" about 1.375 in diameter, with the lack of detail in those cuts I bumped up to 2 inches hoping to get better results. Looks like I can go back and try 1.375 again.

Happy New Year Everyone!

Looks Great Ted!
Some woods just don't have enough end grain accent with the finish!
Christmas ornaments?
NICE!
scott
1.375"D ..........now you're in my neck of the woods:)

GREAT idea!! I like.....

Gas Man, thanks!

Scott: Been in your neck of the woods, often. Always enjoy Maine. Last trip was to Cadillac Mountain. Honestly, I have no idea why I made these other than I saw a post recently by you showing some of your work. Looked like an interesting thing to do so what the heck, give it a go. My better half likes them so she is thinking of putting some of them in a shop her friend owns. Figure I will be working for about a $1.25 an hour, lol. Somehow I do not think that $15 an hour minimum wage is going to reach to my level.

Right now I am working on a leprechaun for an Irish friend of mine, trying to think of something pithy to put on the back side.

The other thing is I want to experiment with this method on some larger carvings.

I have been carving a long time, including hand carving. Sharp corners are what create the shadow lines so the item stands out. These ball nose end mills produce anything but a sharp corner for the shadow lines. Sharp corners are why many carvers try to stay away from sand paper, that, and they hate sanding like the rest of us.

Anyhoo, I am having fun with it.

Oh yea, I forgot to mention. . . that little laser cost about $125. It does not have a power control circuit so it is either on or off. What I do is turn it on at the beginning of the program and just leave it on until the end. The rapid moves leave very faint lines on the work. A very light sanding removes them. One of these days I will spring for a fancier one, maybe. I really do not enjoy fiddling around wiring things up.

They both look pretty good to me Ted, being half blind if there is any error with the dolphins I can't see it

How do you find the Laser to work with? Something I would like to add, was originally looking for the biggest one I could find at a price I could afford but the research I have done so far seems to indicate that the larger the wattage with these blue light lasers the larger the dot size which may have an effect if wanting to do smallish detailed work, more research required

Nice work Ted. I like the combination of carving and laser detail.

Thanks for sharing....

Ted,
Your post is very timely as I am in the process of setting up a laser on my CNC. So far I have been able to make a Mach3 laser post processor for both my tabletop and my rotary. Your G code suggestions are very helpful.

Thanks,

Paul

Ted,
May only be $1.25 an hour, but you love being in the shop.......and doesn't she make you some sort of "Priceless" Cake when you make something she likes?

Yep, Cadillac Mountain sunrises are hard to beat...Unless a busload of Oompah band and dancers show up like one happened to me(After a Midnight ride on the Beemer to make it)
Lived there for 6 months in "Postcard" country, and believe it or not...Ya get used to it, and have to keep kicking yourself to be aware of the beauty!

THOUGHT you might like that John...Laser in yet?
scott

Ted that is awesome.

Never thought about hilighting with the laser.

I have a separate laser machine, I will experiment with some day.

scottp55 wrote:
THOUGHT you might like that John...Laser in yet?
scott

USPS is taking their sweet time....

Very interesting effect - though are you sure your laser has a 6" focal length? Clearly *some* height variance doesn't matter - the pieces demonstrate that. Are you saying you could achieve the same crisp line with 2-3" (or more) of height variance?
Thanks.

I also have a CO2 laser and try to combine cnc and laser as much as possible, manually registering the zero and squareness takes a bit of practice but is worth it. Ted, I see how you earned the Wizard ranking. Thank you Sir.

kaetamer wrote:Very interesting effect - though are you sure your laser has a 6" focal length? Clearly *some* height variance doesn't matter - the pieces demonstrate that. Are you saying you could achieve the same crisp line with 2-3" (or more) of height variance?
Thanks.

About the focal length. Yup, I am sure it is set to 6 inches. It is adjustable, but IIRC when I was adjusting it 6 inches was pretty much the shortest length I could set it to. It is pretty easy to figure out the focal length if it has been changed. What I do is program a 10 inch cut that has the Z rise 1 inch over the travel. Yanno, like G01X10Z1. Then it is just a matter of looking at the cut, picking out the finest line it cut and then measure where that was from the start point. If it was midway then the focus height is .5 higher than where it started. Of course it pays to start out with it manually adjusted to a pretty fine dot to begin with.

As to the height variance. Nah, I doubt that changing the height that much would turn out very well if at all. I am thinking more in terms of about a half inch (which is actually +/- .25 from optimum. In other words I would start with the focus set a bit low to begin with. I dunno, maybe it will work well with +/- 1 inch of height, I will have to give it a shot one of these days.

GeneMpls » Tue Jan 01, 2019 12:39 pm

I also have a CO2 laser and try to combine cnc and laser as much as possible, manually registering the zero and squareness takes a bit of practice but is worth it. Ted, I see how you earned the Wizard ranking. Thank you Sir.

Gene, the way I figured out how to get the zero properly registered was as follows:

Cut a one inch square about a 1/4 deep in some material. I used a half inch cutter with an outside cut. Then I measured the square to make sure the half inch cutter was actually cutting a half inch. I think you get the point behind that. After that I programmed a cut along X axis and gave it my best shot as to where the Y zero should be. Then measured to the edge of the square and moved the Y zero by that amount. Wash, rinse and repeat until that nice little fine laser line went down the edge of the square splitting it in two, more or less. The trick to doing this is to use machine coordinates rather than the workpiece offset display. Write down where the zero was for the cutting tool and then do the math for the difference in the laser location. Geeze, I sure made that sound complicated!

Ahh, while I am at it. . . . checking for squareness. . . . a lot of guys cut a square and then measure across corners with a dial caliper. Bad idea. The square is just fine, but put radii on the corners. Sharp corners on wood do not yield reliable measurements. A radius is much sturdier and is not collapsed by too much pressure on the calipers.

I don't do any of that square cutting stuff to set sqaureness. I attach a piece of scrap material parallel to the base axis (not the gantry) and true it up with a cut. Now I have an edge that is perfectly parallel to the base machine ways. Then I flop a piece of 2 X 4 .25 mdf on the machine against that reference surface. I program two cuts, one about 2 inches from the reference edge and perpendicular to it. I then go to the other end of the sheet and make another short cut. I flip the piece over keeping the same edge against the reference surface and repeat those two short cut a fairly short distance away from the first cuts. Now all I have to do is measure between each pair of cuts. If they are exactly the same the machine is square over 4 feet of travel. If they are different the number is twice the error. My machine is 4 X 3. This also works on an 8' machine. Just buy a piece of 4 X 8 mdf for the cuts and work along the 8' dimension. This method is a riff on the old draftsman triangle trick. It is extremely accurate because it works over the entire travel of the machine. Cutting a 4 inch square and then measuring it with a 6 inch dial calipers will not produce the same degree of accuracy.

About this Wizard stuff: Well, I started as an apprentice and then one day I was a Wizard. But then, a while later I was back to being an apprentice. What is with that I said to myself. It turns out being a Wizard is based on how many posts a person makes. So maybe I am just really a Wizard at being blabby?

Ted,
Have you tried changing these setting to remove the M10/M11 delay?

Whoops!!! Too early in the morning.... Should be M3/M5