So my main goal with the mpcnc is to make signs for the house eventually sell as well. I need to get to practicing first.
Something like this maybe…nothing too crazy yet minus the trees
[attachment file=118796]
I planned on using Inkscape to make everything and then import it into to ESTLCAM as a DXF. The built in font selection on inkscape I believe might reflect whats on your PC. So I would need to get more if you guys suggest something I dont have.
Im quite overwhelmed at the moment since I just finished my build with learning how to use it, tidy up wiring, figuring out feed rates, which cutters to use, what depth, what type of cut, which programs to use, ect.
I purchased a 1/8 45 deg v bit because I was told if you wanna do letters you should be using a v bit. Which brings me to my biggest confusion of the century of what to choose when going with Auto “Carve” in ESTLCAM? I think im really confused as to what does what.
“carve inside and outside”
“carve inside only”
“carve outside only”
Its tough for me to visual it so maybe I need to make 3 different cuts with each setting.
[attachment file=“confused about carving.png”]
The maximum carve width is confusing me as well…if I jack up the number the red lines will get thicker and some come into contact with each other. Is the goal to get that number as high as possible without lines running over each other so the cut looks legible?
The finishing tool…could this be the same 45 v bit but on the last past it takes off less so it leaves a smoother cut? I realize it would be faster with a tool change but im trying to keep it simple and less complicated for now.
If you ever use Comic Sans, you will be dead to me. Even ironically. There is no place for that sort of skulduggery and malfeasance in this community, and I, for one, won’t stand for it!
Just make it readable, and watch your kerning, especially with words/names like “FLICK”…
There may be other ways to do this, but in the preview, you don’t want any circles.
There are two dimensions, the depth limit and the max carve width. If you have small letters, then you can use just the V bit, set the depth limit to something huge and use a single bit. The bit will just trace each letter and go up into each corner.
If you have a wider letter, like the signs you’re talking about you would need two tools. The V bit to do the edges and a flat bit as a pocketing tool. The flat bit will carve most everything, and the v bit will just take care of features that are too detailed for the flat bit. If you are in this area, you’ll need to make the max carving width larger than the width of the letter so the carving can cover the whole area. The main screen will still look like circles, but the preview should show an operation for the flat bit to pocket everything out, and then another operation with the V bit to just tap the corners.
If you’re doing large signs though, you should try it first with just a flat bit and a normal pocket. In order of increasing difficulty it goes:
flat bit and a pocket.
V bit and small enough letters to carve them straight out.
Flat pocket bit and V bit combined to make larger letters.
You might find that the difference between 1 and 3 is negligible and not worth the pain of a tool change, and getting the Z offset right.
I went with the pocket option under holes and parts for the letters. And used engrave on the outer boarder, not sure if that was right choice.
I enabled the finished pass for like .50mm on the pockets and it cleaned up really well and was pretty cool to watch. So that finishing pass just saves my last .50mm from the total depth of cut and runs it differently??
The boarder isn’t 100% center going horizontal on this part and I’m not sure if it’s because I didn’t start my zero exactly on the lower rear corner or it’s something in the program. A quick rip of a table saw would fix it though.
I wanna do a few more signs like this before moving on to vbits and I’d love to know if engrave is correct for a boarder?
Yep. The idea is that there was some force the first time through, so the bit amd machine left more than 0.5mm left. During the finishing pass, there was almost no resistance so it just cleans up that edge. A full depht finishing pass also removes any surface artifacts from multiple passes when you’re cutting deeper.
No, just choose the “hole” tool and add in a pocket. No need to also engrave with a flat bit.
Thanks for the advice its definitely going in the right direction now I feel like. So I might do a few more like this then play with the vbit after. I think I completely misunderstood how to use them.
So say I do that same exact sign all over again in Estlcam pocketing the letters with the end mill I have and I want the edges to have a slight chamfer from the 45 v bit. You guys said I need to a do a tool change (okay fine ill do it lol). Im trying to figure out what would be the most practical way to do a tool without being a big pain in the ass?? Should go back to my zero raise the z in the code and repost another g code for a second cut of just that vbit to hit the edges only. Or should I choose the Vbit in the finishing pass option of my original cut using the pocket options and pick say like 20% of my total depth cut, if I do a 1mm pocket chose .20mm for the finishing pass with the vbit?
So if it works as I posted what the hell is point of carving would it just save steps from what I said above??
Thanks for tolerating all my questions and overthinking lol
You’ll understand what the point of carving is when someone asks you to make something with a script font.
These letters would have to be like 2 feet tall for you to be able to pocket them with a 1/8" endmill. However, if you use carve with a 60* v bit, you could make them 1" tall and they’d look good.
If you look at the corners of the H, you can see how the z axis raised the v bit higher and higher the closer it got to the end of the serif, which makes it thinner and thinner. If it kept going instead of stopping (where it rounds off) it could have gone to a razor sharp point.
Im ordering a 60 degree bit today to try out. Ill have to use my 45 for now though. So stupid question because you bring out a great point that ive been battling since I have smaller workpieces.
What would be a good indicator in ESTLCAM that my letters or perhaps work piece are too small and youll never make out what its trying to carve??
I don’t use ESTLCAM but once you generate the toolpath i am sure you can overlay the toolpath on the graphic you used and if there is no toolpath going into certain places the bit is too big… or maybe estlcam can do simulation where it should give you a 3d model of what it looks like after running the program.
I’ll be very interested in your results and will try to post mine here tonight. I have been working with carving lettering, both pocketing and also outline/island. I have some 45 degree vbits that I have initially checked out and worked with Estlcam but haven’t quite gotten the effect I want. Choosing the right combination of bit, tool path, font, depth and size of the lettering complicating things. Poking around with Estlcamings text and carving features, but still just getting familiar with all the potential parameters that going into this.
And as to comic sans, at least papyrus doesn’t lend itself well to milling, although with a laser engraver on some old paper, you can make great treasure maps!
Im looking at trying out some carving that may involve some pocketing as well so I want to try out checking off the pocketing option with a 2nd tool. Im running a dewalt 660 so a auto tool changer is out of the question lol. Im wondering how will ESTLCAM handle the tool change? Is it going to stop mid cut and I have to quickly change out the tool which if that was the case what would I do about tool height offset for my Z since it will change slightly?? Granted its only wood and I can eyeball the plastic stops on the bits for now.
It can add an M0, which pauses the machine until you click on the lcd.
But what I find is easier is to just take the output gcode and split it into two files. Just copy everything before the M0 to one file and everything after to another file. Then do you tool changing after your run the first and then set up for the second.
The other part is setting the Z height. After you run the first file, you can jog the machine around, change the bit. Then you need to reset the Z. So move the new bit to it’s Z=0 location and do G92 Z0. Then you can jog back near the starting location and run the second file.
So im a little fuzzy on carving with estlcam as to why im seeing a ton of circles if im not supposed to be…whats wrong with it? Bad tool choice? Too small of part or font?
