Mapping cuts for opposite sides of board?

[myxpykalix]

i need a more precise way of cutting this and need advice. So far my measurements and guesses have been pretty good but i need to be more precise with the next one.

I have a plaque that will have text around this round hole for a picture. I will be cutting a 4" round hole all the way thru, then on the opposite side i need to area clear a square to insert a picture from the back. I need to figure a more precise way of cutting the square and round on opposite sides so they match up good so the picture goes in right.

8701

[cabnet636]

i would fix an xy jig to keep resolution the same when the piece is flipped, pocket back first

jim

[john_l]

I just did something like that and I found it best to set the X and Y zero at the center of the piece. Do the pocket first. I also made a couple pencil marks on the table to get registration close.

[bill.young]

Two thoughts...

*) Can you cut both the recess and the round hole from the back? That way they're sure to be lined up.

*) If not, what about incorporating a raised block in your "front cutting" jig that fits the pocket in the back? That would help hold things in place and make sure that everything was accurately positioned, and also let you know if you had accidentally rotated the blank when you flipped it over...if the blank didn't drop down on the block then you would know that something wasn't right. You could cut the recesses and outside cutout anywhere on the table you wanted, and would only need the jig for the front side cutting.

Bill

[myxpykalix]

Thanks bill. Because my piece was way wider then the modeled plaque (for hold down purposes) I didn't have a defined edge to measure from on the sides.
Also because i had writing following the curve of the circle i had to make sure it was in the right place therefore having to cut it from the front.
What i have done in the past is after cutting the circle in front, turn over part then
(for example) I wanted a 4x4" square on the back I would make a + on the front of a 4X4 piece of cardboard, center it from the front as best i can by eye in the center of the hole. Then tape the carboard down on the back.
Draw around it. Measure (as best i can) to the edges and make a new cut file for the opposite side. Think of it like you're hanging drywall and you have to calculate where the plugin is to cut it out. I measure up from bottom, over from side to map out where my square for the hole will be. I've gotten that wrong before!

Anyway i just thought there might be a shortcut way to figure this out more precisely than i have done it in the past.

John,
I always use center for 0,0. It works better for me because i usually leave material on the sides for holddown and then cut it off at tablesaw when finished.
Thanks both for help...

[ken_rychlik]

Jack, Why don't you drill a 1/4 inch hole in the piece in the center. Then drill a 1/4 inch hole in the spoil board at the center of where you want the design. peg it with a 1/4 inch wooden dowel. When you flip it you can't miss. You can glue the dowel in the spoil board and flush trim it when your done.

Kenneth

[grandpaspastime]

One method I use when having to flip a project and cut the other side is a simple one. What ever size bit I use to cutout the profile from the waste. is this. Leave the waste clamped to the table. flip the cutout and for example if I use 1/4 bit. I went to Lowe's, Home Depot and purchased sime soft poly tubing that O.D. size and pack it in the void around the piece where the bit went. resecure to flipped piece down and registration is reasonably close on the reverse side. I do this on making my saddle stands. cutting the mortise pockets for the back, flip the piece and 3d carve the fronts. works for me.

[gundog]

I machine 2 sides regularly. I usually drill 2 small holes in 2 corners .126 or smaller with the bot. Use the mirror image in part Works either flip vertical or horizontal (make sure you flip the sheet to match your choice) you can make those holes in the final cut path so they will disappear when you cut out the part. Write down the coordinates of those holes when the sheet is flipped. I use a laser edge finder and type in the coordinates for the first hole and run the machine to that coordinate move the part until that first hole lines up set a screw in that hole once you have just lined up. Now the part will rotate off the first hole on the screw now find your second spot when it is lined up you have the part lined up mirrored to the front side. It works for me. If you don’t have a laser finder you could carefully use the drill bit to line it up the same way leaving the bit slightly loose so you can move it in and out with your hand.

Mike

[wmcghee]

I would cut the hole out, then clamp through the hole with a piece of wood laid across your part over the hole and a screw or 2 into the table. Then cut outside profile of part. Then, take a scrap piece of MDF or plywood larger than your part. Area clear 1/4" deep or so the shape of the part minus the hole. This will make a pocket for your part to fit in including a boss to stick through the hole. Make it about .005" larger (part that will stick in the hole would be .005" smaller)so your part will fit in the pocket. The use clamps or maybe a small wedge to snug your part and cut the pocket on the back. Make the fixture so you can relocate it easy so you can set it up fast next time.

When drawing your geometry just center your square and your circle to each other and "group vectors". Place them on your profile part wherever you want them and "group vectors" again. Then you can flip and mirror it all you want.

I hope I explained it well enough to understand, I lose track when I'm typing.

[erik_f]

I make peg holes in the spoil board with the bot. Two on one edge and one on the other where the work piece will go. This way when I put my pegs in I can square the piece to the pegs. The corner I want to be 0,0 is a set distance away from my home 0,0. Now I can zero x and y with the normal homing routine and then go to my work piece 0,0 (which might be for example 5,5) and then zero x and y at that spot (for this example 5,5). All I have to do is know the diameter of my pegs and write the file accordingly so when I put my pegs in they locate my work pieces bottom left hand corner at 5,5 (Now my work pieces 0,0). This way you just make two files one for side A and one for side B. Now my drawing can be based off 0,0 instead of trying to find where exactly is some point on the piece or on the table.

[woodworx]

After you machine the first side lay a sheet of mdf down on your table. Use your existing vectors you used for your square and place them where your scrap mdf is laying on your table. Highlight your square and select a "profile" toolpath and tell the machine to cut inside those vectors with a -.04" allowance and cut all the way through your mdf. Take that square out, vacuum out the dust and jam your square down in that pocket. It should fit really tight, and you won't need a vacuum to hold your piece. I guess this is what Wayne said but and area clear takes longer than a profile cut.

[john_l]

This is a nice collection of interesting strategies to achieve the same result. Cool.

[wmcghee]

Your right Justin that way would be quicker. You just would'nt have the boss within the profile to fit up into the hole. You would'nt need it anyway except for maybe clocking your part correctly in the fixture if it would fit more than one way. And you could locate the fixture like Erik is talking about with the pegs for even quicker setups.

[myxpykalix]

Ok These are ALL great ideas and some, in some form or other, that i have used before. I want to get away from making a jig for every cut or project.

Here is what i do now. I have a 90 corner on a piece of mdf clamped to the 0,0 corner. I set my part as depicted.

8702

You can't tell but the mdf has a small lip to hold down the part as well as hold it in the jig. I just screw the holddowns into the mdf wherever I need to.

What I was looking for was a better way to register the hole and square when flipping the part over. Wayne McGhee came closest to what i finally did.
I took his idea of grouping the circle and small square together and mirroring it. However I still wasn't sure that it might be right or it could be moved slightly and you wouldn't know it was wrong because you had no reference to measure against.
So I went and made a big square the size of the material then grouped the big square, small circle, small square all together. Then I mirrored all of those vectors, I can move the big square around and make sure it aligns with the boundry of the size of the part and know for sure the hole is correct in relation to the big square and the small square is correct in relation to the hole.
Thanks to all who gave me some great ideas!

[magic]

I've moved my stops so o.o. is o.o. no matter what bit is installed. Then your piece can be flipped over without making a jig.

And/or, (on a large sheet) The first cut is made then the sheet flipped over. In the program, a rectangle thats 48 x 96 is drawn, mirror the entire artwork and make a new tool-path for the second cut.

Yes the second cut is in a completely different location on the table but if your o.o. is dead-on the strategy works perfectly.

[myxpykalix]

You can't see it but my 0,0 is actually over my indexer bay in open space so that won't work for me.

[gabepari]

Your 0,0 can be anywhere on the table. Mine changes 5 or 6 times everyday depending on what I'm working on. I never move my prox sensors, I just jog to where I want my new 0,0 and hit "Z2". Jack, don't confine yourself to one little corner, it's lonely in the corner


Gabe

[myxpykalix]

gabe, I am like you my 0,0 is whereever i need it. I just meant when i do a C3 and it goes to 0,0 in lower left it is over empty space in my indexer bay as opposed to being right at the corner of the table.
What i do then, because my material 0,0 is in the center of material I do a C3 then drive it to my center. I write down those coordinates then zero x,y wherever that happens to be on the table.

[erik_f]

http://www.lasercenteredgefinder.com/

http://www.iedu.com/DeSoto/SuperZero/

Two ideas that would work for you DeSoto is run by a fellow botter and the rest of his site is very interesting...if you use any of his great ideas shoot him a thank you...he posts some really useful stuff.

[magic]

Never said you can't make your o.o. in the center of the table but being able to place a board in the corner and have the artwork (lower left corner) be o.o. as well..... speeds up my centering time instead of making jigs, especially if I need to flip a piece over.

In the event of carving something onto a cabinet door but you have three sizes, I love pushing the door in the corner and cutting away,

I could see making jigs and attaching them all over the table IF I had more them one spindle working at the same time.

[erik_f]

http://www.talkshopbot.com/forum/messages/27/39746.html?1236693152

[kerrazy]

Jack,
If you are really really attached to your current home position, Just move to a known position from your home location,
Write it down some where then run you file from that location using 2d offset. You have then never lost your home location, and you now have a given location for your fixturing jig.
I have even gone so far as to bastardize my C3 routine, and re write it to move to a different given location for this crazy big jig we use. send me a note if you need more dirt.
I also utilize registration dowels as needed for 2 sided machining.
I would also consider machining finished sized blanks and use a wedge clamp to secure them in place. 3 sides exact location and then the wedge clamp secures the work on the 4th side. easy removal for repeat pieces. just leave the corners open so chips and waste does not build up in them.
I have re-machined many plaques using this method, without damaging the finished plaques.

[mrps]

This is just an idea and have not tried it yet.

I found this post x, y and z zeroing routine (http://www.talkshopbot.com/forum/messages/27/39746.html) over in Accessories and if you leave scrap on each side of you work surface you could:

[myxpykalix]

Dale,
I just saw your response from the 10th. As you can see from my picture depending on the size of the material that Zzero point is always going to be different since I Zzero in the center of the material as opposed to a lower left spot at the edge of the table. So I'm not clear on how doing a 2d offset would be any different then how i'm doing it now.

I can see how that might be advantageous when you have to register and flip parts but i think we are getting to the same place except going about it a bit differently. But please tell me more because many times I think i understand then I go "AAAAAHHHH!, now i get it!" thanks i appreciate the help in understanding.