How to do this?

Hello everyone I am looking for ideas on how to do this project over and over again very easily.

here is the project

I want to be able to cut a whole bunch of circles out before I take it to the machine to do the engraving

I am looking for ideas on how to make a jig to not only clamp the circle in place but also zero my machine in x, y, and z easily and in the same place over and over again

I have to aglin the slots on the back with the #12 on the front

here is a picture of what is on the back

does anyone have any ideas on how to do this on a production scale I am open to all ideas please let me know

thanks for your help guys

edit: I am thinking that it is possible to not cut the slots before the engraving so I wouldn’t have to align the slot to the #12 in the machine I can just place the circle into the machine cut the engraving and then cut the slots on my router table later

also I am using universal gcode sender for this operation not easel

also here is a picture of a clamp that I did think of but it does not help with zeroing the machine

take a look:

To zero the machine, can you mark the center of your work where the clock mechanism will be and use that as your work home?

the problem is there will be a hole in the work piece right where my x, y, z zero is at

Get some good double-sided tape to do the hold-down and you’ll be fine.

Is there a reason you couldn’t engrave the clock face first and then cut the circle? I’m assuming you’re cutting the circle with something like a router circle jig. You could have the engraving bit mark where the center hole should go while it’s doing all its other work. Once you take the engraved piece off the mill, drill through where it marked center and cut out the circle.

@NicholasKoza

yeah the problem with that is each clock will be different and I am doing a production run of 100 so I would like to cut all the circles at one time and them have them ready as orders come in so all I have to do when a order is placed is to engrave and finish

What about a dowel in an mdf template… the template clamps to the surface in a known position and the dowel comes through the blank’s center hole.

@ErikJenkins

that would work but how do you setup universal gcode sender to remember x, y, and z zero position if the blanks are cut days, weeks apart?

1 Like

Zero on the corner of the template. Accurately measure the center X and Y offset. Offset your center with a macro in UGS, it will be the same each time.

1 Like

@ErikJenkins

yeah i have never done that but i need to learn it

I am curious what do you think about jus using a vacuum table to position the circles each time?

1 Like

I don’t use one, but it would work.

I just thought of something. Would this work? I’m no expert, so forgive me if this is dumb.

First do the backs on your router table like you said, and cut a block that just fits inside the pocket for the mechanism and is flush. Then glue that to the center of a piece of wood that is slightly larger than your clock. Run a bolt up through the middle that will fit the hole for the clock hands, and affix the whole thing to your x-carve.

That way, as you remove each carved face, you could just drop a new one on and affix it with a wing nut in the center. The block will hold it in the proper orientation.

@BradT

well in theory that would work but i see a possible problem

btw not a dumb Idea

the center square hole for the clock movement will be round on the production clocks (sorry that is my fault I didn’t tell you that) this shouldn’t be a problem

but the problem that i see is the tool paths cross the center of the clock and would hit the bolt in the center and even in fusion 360 I am not sure that there is away to make sure that the bit never crosses the center of the clock. the software that I am using to generate the v-carve is F-engrave and I know that its impossible to avoid the center area with the tool paths

does anyone know if V-carve pro has this capability??

the only way I see to avoid the center is to raise the z saftey height and with it being a v-carve that bit would be moving up way to much and increase the time the total engraving takes

but its not a bad idea and is on the right track its just hard to hold something down that cannot be clamped top side

also double sided tape would not work because I would like to get a jump on finishing the back side of the piece before the engraving so I think that the tape will cause an issue with the surface finish

For setting up the CNC you can use work coordinate systems for milling both sides. http://www.shapeoko.com/wiki/index.php/G-Code#Using_the_Work_Coordinate_Systems

Not sure if you have limit switches, but WCS come in real handy with limit switches. send $h to home

I would build a small jig for clamping/work holding. Starting with square material you can use wedges to clamp it in place. Have the cnc mill out the back pockets, center hole, and cut the circle. Save your zero to the G55 work coordinate, and then when sending make sure your file targets the G55 WCS.

Once you have the first side cut out, you can flip the piece and use a screw in the center hole to hold down the material for the face cutting. Use a different WCS (G56).

You could batch out a bunch of the back side milling first using a 1/4" end mill and then batch out the other side using a vbit.

The WCS will keep you accurate in the X and Y. When changing a bit you will need to adjust the Z.

Can you use the center of the work as your Zero point? If you make a jig with a short enter dowel that the clock face would drop onto, you can get repeatable results.

Make your jig out of something with a sharp corner so you can always put it in the same spot on your machine. Mount a dowel to it that does not stick up higher than your clock face. The center of the dowel will be your X0 and Y0 locations.

This next part only works if you have limit switches and have a repeatable machine home position. GRBL will let you store multiple workpiece Zero locations. The G54 through G59 commands change these locations. G54 is the workspace (material zero) the machine defaults to after a power cycle or reset. You can use one of the others as your Zero point so you can come back to this project whenever you want.

I did a forum post about my investigations into this a while back. Here is the link.

EDIT: I saw @FrankWiebenga post pretty much the same thing as I was writing this up.

You can set the safe retraction distance in Fusion 360 (I think that’s what it’s called). It will add a little bit to your carve time, but it will make sure the endmill rises enough to clear obstacles.

EDIT: In F-Engrave, it is your Z-Safe parameter on the main screen. It raises the bit a certain level above the stock before any rapids.

In 360 there is an option in the cutting parameters for the operation to set a ‘fixture’. You can then select some geometry that it will avoid while doing the cut.

@EmilianoMolina

thats awesome could you tell me how to do that?

unfortunately fusion 360 cant v-carve for this project

but I would like to know how to do that for the future on other projects

Here is a link to a video that shows you how to set it up:

BUT! I’m not sure that it works like I thought it did. I assumed that it avoided the fixture, turns out it may only use it for letting you know if you hit it. If you want to avoid it you may have to set up the fixture as ‘model geometry’ instead:

https://forums.autodesk.com/t5/ideastation-request-a-feature-or/fixture-avoidance/idi-p/5721871

Instead of having the machine cut the center hole, have it engrave a small x. Zero to that each time.

Drill the center holes by hand after they are finished.