Thank you I will look into that for sure
The center hole will be drilled by hand all I want to use the X-carve for is the engraving
If you have limit switches the G54 solutions mentioned above are really good.
Do you have limit switches?
Use your machine to make something like this and use it to find the center of your circles. Mark with a pencil. Then clamp down and zero to the center of the circle.
hey jdm the circle, clock works relief and center hole will already be cut prior to putting on the x-carve the x-carve will only be doing the engraving. I am trying to find the best way to hold the circle to the table and find a repeatable x, y, and z zero
oh yeah I have limit switches on my machine that would be good I think for zeroing the x, y axis and then manually do the z height I need to read up on what you are saying
I think the combination of that and a vacuum table with fixture should solve my issue
If you have limit switches then you only need to be able to set the fixture in the same place every time. Use the G54 method described above to zero in on the fixture reliably after homing the machine.
If your stock height is consistent then it will also work on the z axis!
@Zach_Kaplan can verify that I have developed a mass production system with X-Carve that works well and I will share some ideas with you here.
I do a lot of mass production work on the X-Carve on a daily basis. Thereâs a few tricks to get this to work quickly. My work involves a bit change during each piece as well. One of the first things I have to say is you need to minimize the number of steps involved in your workflow and also minimize the number of times youâre clamping material onto your machine. So my first question is, why would you cut that out first and then put it into a jig to carve on the X-Carve? Youâre handling the material at least twice and you donât need to. Use the X-Carve to make these cuts for you.
You need to modify your X-Carve and build an X and Y rail for each work piece to butt up against. The lower left corner should be your zero point, but donât put the rail all the way to zero. You only need to start the X and Y rails about 2" from their respective zero point. That way, you can still move your bit to 0,0,0 (x,y,z) and also clamp your material close to the lower left corner without the rail getting in the way at 0,0.
One of the best ways to square up your rails to the X and Y path of the X-Carve is to get some 1/4" dowels and use the X-Carve to drill about five, 1/4" holes in your waste board along the x = 0 and y = 0 axis. Put the dowels in the holes and butt your straight rail (wood or other material about 1/2" in height) up against the dowels and screw the rails into your waste board. Do the same for the other axis as well. Youâll then have squared rails along the x and y axis.
When you start carving material, I would start with a piece of material big enough to to cut your clock out from. I would carve the clock face and the customized part of it in one or two tool paths as needed first. Mount a SQUARE piece of material up against each of the rails mentioned in the previous paragraph. Adding these rails saves a ton of time when youâre using your X-Carve for mass production. Every time you put a square or rectangle piece of material against both rails, simultaneously, it will automatically be squared with the X and Y axis on your X-Carve because youâve already created that jig above.
After those cuts are made, bring your bit back to the home position (X, Y) and move the Z about an inch above the material. Change your bit as needed and then while the bit is still loose enough in the collet of the router, lower your router in 1mm steps to the work surface as the bit slowly pushes into the collet as the router moves down toward the work piece. When youâre at the proper height (meaning the bit is on the work surface and the router has taken in enough of the bit shaft) tighten your bit while itâs on the surface.
At this point, reset zero in UGS, or confirm Home in Easel and run the next tool path. Repeat the process for each tool path you need to cut. Finally, repeat this for the final cut, which should be the outside of your clock. This should be your final cut to remove it from the material stock.
In summary, 1) youâve minimized the mounting of the material to your X-carve, 2) you automatically squared up your material at the start by butting your material up against the x and y rails explained above, 3) you only need to reset the z whenever you change a bit, and 4) your final carve cuts the clock out of the material stock. All of this while only handling the material once from start to finish.
I will be producing some videos in the near future that explains this process as well as other mass production tips. Furthermore, Iâll be creating some videos on how you can make some serious money with your X-Carve.
WW, what I am suggesting is to drill the center hole as the last operation with a drill press or hand drill.
hey thanks for that long post I am going to read everything in detail and look into that I like your ideas
here are some of my thoughts really quick
I have been testing cycle times per piece and currently I am sitting at 28 min per piece with 1 tool change and 1 material flip
the actual engraving takes about 14 min so I am looking for way to reduce my time to not much over 18 min for total machining on piece as it is 18 min working 8 hrs a day is 4 days per 100 and thats not including the time for setup, tool change, and material flip
So my thought was as follows
- Cut my board material into 12x12" squares with miter saw (5 seconds)
- use template to place on square and pencil the outer circumference of circle and the center point (10-15 seconds)
- Drill 1/8" hole in the center of square board with hand drill or drill dress template (10 seconds)
- Place square on router table with a pin through the center hole offset 5.5" from router bit spin material to make a 11" circle (1-2 min)
- Lift circle off the router table and take to drill press clamp into circle fixture and drill out center hole with a 3" Forster bit with 5/16" centering drill bit (30-45 seconds)
- take to X-carve and place in vacuum plate fixture zero machine and engrave(14-18 min)
- Take piece off the X-carve and take to router table with keyhole fixture and use keyhole bit to make the keyhole cut on the back side (30 seconds)
- Done (21 min 45 seconds)
Also running the X-carve on a production scale cutting 3/4" oak will be hard on the machine
this is just my opinion and correct me if I am wrong but the x-carve is just not a production machine to be doing this operation all day everyday for 10 hrs straight. I have problems with my X-carve with the dewalt router getting a nice cut at 55 inch/min at .110 doc and 16,000 rpm really 55inch/min is just to slow and to hard on the router bits thats no where even close to the proper chipload for the tool all I will be doing is spending alot of money on bits and time on machine maintenance running it like this
that would work angus but the clock movement relief will be round not square in the production clocks
@PhilJohnson
if you dont mind what type of material do you make your clocks out of and what kinda volume do you do?
do you find it hard on the machine to cut all of that out over and over?
do you have a cycle time per clock?
I do like what you made in easel to hold the clock thats interesting but i couldnât get the link to work?
oh yeah those look pretty good
curious why donât you just buy 12" wide poplar? (well its like 11.25" when you buy dimensional lumber but would work for your 10.75" clock
I am just curious because I thought about doing glue ups but with the added time and glue expensive I didnât see the benefit I buy lumber by the board foot so I donât see a cost advantage either
Also do you use 3/4" thick poplar? I just ask because the thinnest clock works that I could find was 5/8" so that will a flush relief in the back side that only leaves me 1/8" to mount the clock works how do you recess the washer and nut in your clock?
what are your thoughts?
Homing switches and G10 command work perfectly for me.
I can give you a step by step, if you think it will help.
i would love that take me to school!!!
me and my client are bringing a product into production and to get costs down we have to do a minimum order of 100 thats all the details I can really give on that its an investment for sure
1 Like
Ok, Iâm not in front of my X carve right now, but I think I can give the basics from memory.
This is all done in UGS, but as long as you have an accurate position display, youâre good.
Home you machine, then set all your axis read outs to 0.
Move your machine to your desired X Y origin. Note the coordinates somewhere that you can refer to.
Then (in UGS) type G21( metric positioning, since my readout is in metric, even though my programs are in standardâŚ) G90 enter. Should get an OK.
Then type G10 L2 P1 X----- Y ----- Z------
This will store your X Y and Z at work offset G54. Your Z should be a negative number if you are touching off the material as you set your origin. Donât need the Z, but if the 100 parts are all the same, why not?
Now in your program, all you have to do is tell it G54 X0 Y0, and you should be move to the origin, exactly.
If youâre using standard ( rather than metric) make sure to change the G21 to a G20.
The G54 is modal, which means all positioning moves are based off that, until you call up another offset.
I set G59 at the upper left of my part, and send it to G59 X0 Y0 at the end of the program, to remove parts. If you do that be sure to type G54, to switch work offsets before the next program.
strong text
$7 a board ft or linear foot? You are buying the panels glued or are you gluing?
Iâm in my shop 8-10 hrs everyday and the x-carve is running most of the time, just stopping to set up new cuts, so for introductory small shop production, I would say I have been impressed with how much it accomplishes.
I run hardwoods, mostly maple (a bit harder the oak). I started out real gentle with my feeds and speeds, but after doing the mod on the gantry Iâve been slowly climbing up. I do full depth 4 quarter (1") profile cuts and right now am getting good cuts at about 55in/min. at .08" doc with a 1/4" spiral. A smooth finish and tight accuracy are really important for my pieces.
With the chatter Iâm currently getting I wouldnât feel comfortable cutting much faster than that, but you may have a tighter machine than me.
As far as your jig I think these guys have you set with good advice there. My only thoughts are I always use a bumper board on the bottom and when I finish a job I jog the machine up 15" switch out my work piece and then bring it right back. So my x and y are already set and I just adjust the z.
Good luck!
3 Likes
drill and Put a Dowel into the center of the piece, that way the router can pass through the center. It shouldânt matter what position the Round Blank is in. set up another Hole is you Waste board for alienment of the blank.Use double sided tape to hold the blank down.
Full 1" depth cuts? How much material are you removing? Doesnât the X carve flex too much for that? Please share.
I believe he means final depth is 1" but cuts at a .08" depth of cut per pass lol no the x-carve will literally brake apart if you try that in hardwood but you could do it in foam all day long!!
1 Like
I have been cutting Red Oak @ .1" depth cuts (total .5") on mine, but I tweaked my motor amperage and Modded out the belts a little to have a more consistent tightness. Iâve run thru about 40 of them now, and itâs working fine. My Feed rate thro is only set to 34⌠I would love to know how I could get it up to 55⌠Hell, If I could get it up to 40, I would be happy, but I worry that I might skip a bit. Would like to know what @JosephCompton did on his to get that kind of cutting speed.
are you using a .25" bit?
I run mine at between .1-.06 doc all at 55 in/min in red oak using a 2 flute O-Flute down cut spiral mill The O-flute is easier on the machine and will cut soft woods like a dream!!
also you might look into a high speed steel bit for some natural woods as they work awesome in some cases
1 Like