Router Forums banner

1 - 20 of 21 Posts

·
Super Moderator
David
Joined
·
3,569 Posts
Discussion Starter #1
Late last year a friend asked if I could cut a sign for his son-in-law's new business. I was more than happy to do that so he brought the piece of wood by the house and it's been sitting in the shop since then because there were quite a few projects ahead of it (the Curly Maple and Walnut cross being one of them). So yesterday I put the Pecan slice up on the work table to begin mounting it on the CNC.

The piece of wood is from a Pecan tree that had to be cleared from the property before the building could start so this has a bit of sentimental value for them, maybe more nostalgic than sentimental, but either way I have one shot at this. When we first talked he just wanted the name engraved into the Pecan slice. The second time we talked they decided they wanted the logo as it is on the business card and for that to be raised from the surface. Now, in concept anyway, I understand what needs to be done to accomplish that but I had never done it.

I worked through setting this up in Fusion 360 for what seemed like days - an hour here, two hours there, etc. - and never got comfortable with the generated toolpaths. In the setup for cutting this was leveling the face with a 1.5” bottom clearing bit, about 6 minutes, and from there it got complicated and difficult. In Fusion 360 when I set up the next bit, a 1/2” flat bottom bit, to begin cutting away everything except the logo and letters I never could get the geometry correct. When I got it to a point where it was acceptable the cutting time was over 2 hours and I just didn’t think it should take that long.

When I switched to a 1/4” bit to cut what the ½” bit couldn’t get to the time doubled – over 4 hours. No matter how I set the parameters I couldn’t get it set to only cut what the 1/2” bit couldn’t get to even though I had “from previous operation” selected. It wanted to cut the entire piece as though the 1/2” bit was never involved. When I switched to a 1/8” bit the time was truly ridiculous!

I finally turned to the Fusion 360 community where I gave them my files and noted the issues I was having. A gentleman there took the project, reworked my files, and sent his version of how the CAM portion should be set. He did some things in the setup that I still don’t fully understand but they seem like they’re going to work.

So here are some photos and minor progress; this is the slice as delivered -


Logo and name from their web site -


I used CorelDraw to overlay the proposed letters and logo for approval. One thing I had to work around is the void in the center -


The initial toolpath for the 1/2" bit follows the approximate outline traced from the photo. Turns out this isn't entirely accurate but at this point, since I didn't draw that outline (the guy from the Fusion 360 community added that and I can't seem to edit it), what this doesn't cut will be a tiny bit on the perimeter so I'll just finish this by hand when it comes off the CNC machine -


Here's the toolpath for the 1/4" bit, cutting only what the 1/2" bit can't get to -


And ditto for the 1/8" bit, cutting what the 1/4" bit didn't -


One step that was necessary from the start is that I had to draw the logo. I drew this in CorelDraw and exported it as an svg file to import into Fusion 360. I had to keep modifying it because even a 1/8" bit wouldn't get to the entire logo. As it is I'll finish the tiny openings near the bottom with a Dremel, 1/16" bit, and router base. I can control that pretty easily but don't want to risk breaking my 1/16" bit for two little holes.

Fixing mounting boards to the bottom of the Pecan slice -


Verifying it is close to level so I wouldn't have to take much off for surfacing -


You can see how large this is relative to the CNC. The CNC frame is a Saturn 2' x 4' from Fine Line Automation but the actual cutting area is 26" x 50". The Pecan slice is 25 7/8" across at the widest point. No problem, right? Wrong! When I did the surfacing profile in Fusion 360 I didn't count on the machine needing turn around room a the end of each pass. The loops at the end of each pass pushed the X axis right into the bumpers and tripped the sensor. So I moved the starting origin point for X about 1/2" to the left but it made no difference. Fortunately the sensor stopped it before crashing into anything at 600 ipm. I toyed with it for a while and finally had to go back into Fusion 360 and tell it the piece was only 24 3/4" wide and then it cleared by 1/8". Since it was only the facing operation and I could see it was going well past the perimeter and it wasn't going to be a big deal, I would just change it back for the letters and logo.


Once I was comfortable with the clearance, having run it about an inch above the Pecan slice to make sure, I set zero, fired up the spindle, and hit go. Two things became apparent right away - 1) even though I had the dust shoe on and DC going, tiny Pecan chips were going everywhere and, 2) the large flat bottom bit didn't like climb cutting at all. It was burning on each pass that was climb cutting but clean on the conventional cutting.


Back to Fusion 360 to change the toolpath to only cut conventional (no loops at the end, rather it raised the Z axis and went back to the other side to cut in one direction only for each pass) -


These tiny little Pecan chips were all the way to the window 15' away, down my shirt, in the keyboard, even under the CNC machine!


This came out much better and took a few passes but it cleaned up nicely. You can see the lines along the X axis but it is very smooth. It will all be cut away in the next step anyway -


I think it's a pretty piece of wood and with a little sanding should look pretty nice. I have two other jobs that need to be finished by Tuesday so I may pull this off and move on to those, then mount this again for the letters and logo. At this point it won't matter if I take it off but once I start the letters and logo I can't move it, so instead of getting backed into a corner this will probably come off tonight.

More later -
David
 

·
Registered
Joined
·
4,352 Posts
I've said it before and I'll say it again. Other than just cutting text in material - THIS IS NOT A FAST PROCESS!!!!!!. My Last Supper carving was on a 24 x12 piece of 5/4 pine --- 5 hours for the rough cut with a 1/4" end mill and close to 9 hours with a 1/8" ball nose - just to get all the detail in. A 3/16 bn may have worked and saved a little time. Could have used a bigger end mill for the rough cut, but the 1/4 got more material out. The less material the finish bit has to take out, the smoother and more detail it produces. Aspire also would have probably saved you a lot of time in the design and file stage.

Think about Vegas in Oct David-- good weekend away with Mama and learn a little more what Aspire can do, since you're going to be getting it anyway, at some point.

I hate having only one chance when someone provides a special piece of material. So much can go wrong. Unless it's something that I know will work, I usually cut it on a test piece first, which really adds to the time frame. At least on a "custom" order with your material, if you screw up, you just get another piece and start over. All you're out is some time and a little material. But mess up a sentimental special hickory piece brought to you by a fiesty little old lady - you sweat a little.

It's all a learning experience, my friend. Never stops!
 

·
Premium Member
Joined
·
17,426 Posts
David I'm with you as that is a pretty piece of wood , and almost a shame to engrave into .
Can't wait to see the outcome though ;)
 

·
Super Moderator
David
Joined
·
3,569 Posts
Discussion Starter #4
I've said it before and I'll say it again. Other than just cutting text in material - THIS IS NOT A FAST PROCESS!!!!!!. My Last Supper carving was on a 24 x12 piece of 5/4 pine --- 5 hours for the rough cut with a 1/4" end mill and close to 9 hours with a 1/8" ball nose - just to get all the detail in. A 3/16 bn may have worked and saved a little time. Could have used a bigger end mill for the rough cut, but the 1/4 got more material out. The less material the finish bit has to take out, the smoother and more detail it produces. Aspire also would have probably saved you a lot of time in the design and file stage.

Think about Vegas in Oct David-- good weekend away with Mama and learn a little more what Aspire can do, since you're going to be getting it anyway, at some point.

I hate having only one chance when someone provides a special piece of material. So much can go wrong. Unless it's something that I know will work, I usually cut it on a test piece first, which really adds to the time frame. At least on a "custom" order with your material, if you screw up, you just get another piece and start over. All you're out is some time and a little material. But mess up a sentimental special hickory piece brought to you by a fiesty little old lady - you sweat a little.

It's all a learning experience, my friend. Never stops!
Fully agree, John. The good thing, that I forgot to mention, is that I now have the total machining time down to about an hour - about 23 with the 1/2" bit, 12 minutes with the 1/4" bit, and about 22 minutes with the 1/8" bit. That's not too bad for something of this size. The letters are 3/8" high so that's a fair amount to take off when you can't just plow it off with a leveling bit.

It's just like mowing a yard with no trees vs. a yard with lots of trees. You can cut the yard with no trees with a large mower in no time but the one with lots of trees requires a smaller mower and takes a lot more time but sure looks better than the plain old bare yard.
 

·
Registered
Joined
·
834 Posts
I know absolutely nothing about CNC work. But, you have my attention and I am awaiting the results of this project.
Thanks for posting it.
David
PS: I plan to get me a CNC when Stick does.
 

·
Registered
Oliver (Prof. Henry)
Joined
·
2,193 Posts
A great project. I'm looking forward to the next installment.
 

·
Super Moderator
David
Joined
·
3,569 Posts
Discussion Starter #7
Finally got back on this to cut the letters and logo. I have one small area I'll do by hand, well, with a Dremel and router base anyway. At the bottom of the medical symbol there are two small recesses requiring a 1/16" bit and I didn't want to mess with that on the CNC. It won't take 5 minutes with the Dremel.

Finished for all practical purposes -


Even with the dust shoe in place we ended up with Pecan chips everywhere!


I'll cut the two small recesses tomorrow and may post another photo, if I have time I'll do a video on this, as well.

Thanks for looking at this little project!
David
 

·
Registered
Joined
·
4,352 Posts
Way Cool, David.

How many passes and at what depth was each one.

Doing raised letters with wood is always a crap shoot. Sometimes, they don't come out so good. Now you can exhale.
 
  • Like
Reactions: difalkner

·
Super Moderator
David
Joined
·
3,569 Posts
Discussion Starter #10
Way Cool, David.

How many passes and at what depth was each one.

Doing raised letters with wood is always a crap shoot. Sometimes, they don't come out so good. Now you can exhale.
With the 1/2" bit I took two passes at 3/16" each, 200 ipm, cutting time was 23 minutes. Next was the 1/4" bit to cut just what the 1/2" bit couldn't get to, cut 1/8" deeper with each pass - could have been more aggressive but it would have only saved a couple of minutes and increased the opportunity to rip off a corner here and there. I ran the 1/4" bit twice at about 12 minutes each. I purposely set zero about 1/32" too high on the first run because I didn't want to cut a trough around each letter if I had accidentally set zero a few thousandths too low. So I ran it once and then measured how much I needed to lower zero to cut flush with what the 1/2" bit had cut. Next was the 1/8" bit and I did the same thing with setting zero too high on the first pass.

I've only cut raised letters twice, once on face grain and now on this Pecan slice (end grain). I have to say cutting raised letters or a profile on end grain is a breeze compared to face grain - no tear out, letters are crisp, but lots of chips flying around.

It's probably time for me to check into building an auto zero touch plate. Eyeballing it and using a piece of paper under a bit to determine zero is a weak link in my process. :surprise:
 

·
Registered
Joined
·
4,352 Posts
Z-pucks weren't available yet when I got my machine. I just use a playing card. Good nuff for what I do. And it does let me cut a little deeper or shallower, depending on the look I want.

If (and when) I get another machine or update this one, I probably would get a Zpuck.
 

·
Super Moderator
David
Joined
·
3,569 Posts
Discussion Starter #12
Z-pucks weren't available yet when I got my machine. I just use a playing card. Good nuff for what I do. And it does let me cut a little deeper or shallower, depending on the look I want.

If (and when) I get another machine or update this one, I probably would get a Zpuck.
I'll probably design and build my own. As simple as it appears, $120 seems awfully pricey for the Z-puck. If I was going to spend that I think I would add $10 to it and get the Auto Z and corner finding touch plate from CNCRP.

I'm like you, though, in that I keep paper and business cards handy for setting zero and it's been ok but certainly isn't precise. A V-bit will poke right through either one with no problem at all.

I prewired everything when I built the enclosure so all I have to do is plug in the touch plate to my remote E-stop box (often seen on top of the enclosure in my photos and videos).
 

·
Super Moderator
David
Joined
·
3,569 Posts
Discussion Starter #13
Had some time this afternoon and cut the final two pockets on the logo -


Logo up close -


Completed sign -


Thanks for following along!
David
 

·
Marine Engineer
Doug
Joined
·
4,783 Posts
I don't know if you touched on it in the other post, but how are you going to finish this to ensure that there isn't any more checking? It would be a shame for a beautiful piece like that to wind up with a huge crack down the middle.

(I am afraid to push my machine anywhere near the speeds you run yours!)
 

·
Super Moderator
David
Joined
·
3,569 Posts
Discussion Starter #15
I don't know if you touched on it in the other post, but how are you going to finish this to ensure that there isn't any more checking? It would be a shame for a beautiful piece like that to wind up with a huge crack down the middle.

(I am afraid to push my machine anywhere near the speeds you run yours!)
I talked to my friend who asked me to do this and he's going to just put a clear finish on it - Varnish or Poly. At first he planned to paint it but I told him if that's still his plan then he can't have it back - LOL!

The speed I run is slowly creeping up. Several months ago 100 ipm was my cap but the more I push that envelope and see things working fine the faster I want to try and go. When I made the initial 1/2" bit cuts on this at 200 ipm I was thinking the whole time I could have gone to 250 or even 300 with no problem. Maybe next time I'll try that.

David
 

·
Premium Member
Joined
·
17,426 Posts
I'm amazed a letter didn't chip out as it was doing the fine details ? I'm sure a newbie like me could never pull this off .
That's certainly one of the nicest signs I've seen David , great job :)
 

·
Super Moderator
David
Joined
·
3,569 Posts
Discussion Starter #18
I'm amazed a letter didn't chip out as it was doing the fine details ? I'm sure a newbie like me could never pull this off .
That's certainly one of the nicest signs I've seen David , great job :)
Having seen that piece of wood in person, I can truly say it is beautiful. Even more so now that the carving is complete.
Thanks, Guys! Fun project, for sure.
 

·
Premium Member
Joined
·
17,426 Posts
David , am I misunderstanding things or did you finish off with a dremel ?
If so , could you not have put a really small bit in your spindel and had the cnc do it?
 

·
Registered
Joined
·
3,723 Posts
Cutting end grain normally yields nice clean cuts with little or no tear out just like David says. I do inlays in end grained cutting boards and you would be surprised how well end grain cuts. I leave uncut pieces in the pocket sticking up that are slightly larger then 1/16" diameter and the inlay has a matching hole. I have never broken off any when installing the inlays. The grain running the depth of the the board instead of across the board make those small pieces stronger.

Rick the problem with the smaller diameter bits they also have a smaller depth of cut. Most of the 1/16" bits have a cutting length of 3/16" but if you look around there are a few with 1/4" cutting length. The ones I use have the 1/4" length and are American made(Wolf brand).

David love that sign!
 
  • Like
Reactions: difalkner
1 - 20 of 21 Posts
Top