Machining both sides of material

[cnc_fabricator11]

Hey everyone,

I have a PRSAlpha and I'm having difficulty aligning circular cuts on both sides of a sheet of MDF. The process thus far has been cutting the circles on one side, setting a jig to the outside corners of the material, flipping the material, and then cutting the same circles on the other side. For some reason the circles aren't lining up and I'm getting a small lip on the cut as if the circles are shifted offset from one another (see attached photos). The strangest part is that the circles towards the middle of the material have the largest lip, while the circles on the outside only have a tiny lip. I've checked the drawing file to make sure it was symmetrical, I've made sure our table is square, we've tightened the x motors to ensure that they aren't slipping, and the material is being placed in the jigs in the exact same place when flipped but no dice. If anyone has any other suggestions I would really appreciate it.

Thanks,

-Pat

[myxpykalix]

Let me ask a stupid question. Why are you using a cutting toolpath like that? Why not cut it all the way thru from one side?

Get the right type of bit so as not to blow out the bottom (thats a question for some other expert...).

What is the waste material here, the circle cut out of the center so the important part is the piece with the hole? You could get some sacrificial material under the plywood and cut the hole deeper then the material and with the right bit you should have no problem.

[knight_toolworks]

I was going to ask the same thing. I think it is the roundovers but it's faster to cut them on a router table or with a handheld router.

[hespj]

How about instead of a jig which holds the sides of the material you make a jig with a few circular upstands which fit into the partial holes you've cut?

John

[cnc_fabricator11]

Thanks for your responses. Jack, we're trying to achieve a roundover profile on each circles edge on both sides. Sorry I forgot to mention that in the original post. We considered using a handheld router but would like to accomplish this on our CNC machine if possible. I'm sure we will encounter the same problem on future projects that require machining from both sides so we would like to come up with a solution on this particular project.

Thanks,

-Pat

[jerry_stanek]

Unless your material is exactly square and the parts are exactly centered and you place the piece in the exact same spot on the table you are going to have problems. Even the swelling of the wood will make your cuts off.I have cut some stuff that the change in temp during the cut caused the cut to be off.

[bruce_taylor]

When you flip the sheet it comes off a different edge you may have to mirror your piece to get it to line up correctly, Ihave done this successfully but I set up block and cut the edges then mirrored the cut and placed it at the rights place to make it work. Good luck.. it does take a little to get your mind around it to make it work but it is possible with a little tweaking, only worth the time if you have a few to cut though.

[beacon14]

A relatively simple way to do this is to make your jig slightly oversized, say 1/4" wider than the board. Place the board against the right side of the jig to cut the first side. Then flip the board and place the same edge that was against the right side of the jig, against the left side of the jig - that way you are always registering from the same reference surface.

The best way to make the jig is to place it on the table and have the Shopbot machine the sides that the workpiece will register against. That way you know the jig is referenced properly on the table.

You will have to offset the second side vectors by the 1/4" to make up for the workpiece being shifted. I hope this makes sense. Once you correlate the jig locations and the vectors for both sides it's easy to cut multiple parts without having to put extra holes in the workpiece for registration, or use a different jig for the other side.

[knight_toolworks]

Thanks for your responses. Jack, we're trying to achieve a roundover profile on each circles edge on both sides. Sorry I forgot to mention that in the original post. We considered using a handheld router but would like to accomplish this on our CNC machine if possible. I'm sure we will encounter the same problem on future projects that require machining from both sides so we would like to come up with a solution on this particular project.

Thanks,

-Pat
the thing is it takes far more time to do it all on the cnc. If you just cut the full sheet out and while another is getting cut you round over that one you cut the cut and setup time in less then half. That lets you get the part made faster.
the easy way to do this is the cut the part slightly large and drill holes in each end. your jig will have matching pegs. you cut one side flip over and use the page to center it again. The problems with this is holding the part in place well. You can do one sheet by rounding over one one full sheet drill the holes and chop the sheet up then do one at a time to do the second side and all the slots.
But any method will cost you time and drive you nuts in trying to get the material perfectly flat for a good roundover.

[twelchPTM]

Harvey Tool has back corner round endmills (I'm sure other manufactures do to) It may take a few tries to get the toolpath right but they allow you to round the bottom edge of a part with out flipping it over. I think you would have to add a "tail" to your profile cut and allow clearance for the backround to go into the tail before moving up against the part. It probly would take a little longer to do it on the bot then going old school and using a router but if the bot is doing the work your fingers don't need to approach the whirling blade of death, and you can get other things done so your not really wasting time.

[dlcw]

Like Steve says. I cut 4" circles and ovals from 1/4" MDF all the time and take the parts to the router table and round the edges while the next sheet is cutting. I do the same thing with larger circles, ovals and football shapes I cut from 1/2" MDF. I thought about trying it on the CNC but figured I could do it faster at the routertable then dealing with the flip operations at the CNC.

To accomplish flip operations, you need to create an exact mirror image of your vectors. You also have to have an EXACT size for your material. And I mean dead on. The original side vectors should be centered in the material. The flip side with the mirrored vectors should also be centered in the material. Then you need to have a registering system on your table that enables you to position the material in exactly the same position when you flip the sheet. For those that do flip operations with SBLink for cabinet parts, we deal with this all the time.

I'm about to cut several dozens sheets of sign letters on laminate on MDF substrate using flip operations to stud mounting holes and write sign numbers on the back (using Widgetworks pen system), them flipping the whole sheet over, beveling the letter edges and cutting out the letters from the front side. I have indexing pins (SBLink) on my CNC table that enable me to register the sheet in exactly the same spot for the flip operations. It is time consuming and tedious but I have about 800 letters to cut out ranging is size from 1.5"x1.5" square up to letters 52" tall.

[cnc_fabricator11]

Thanks everyone for your suggestions. After testing out several ideas we've decided to approach it per Steve and Don's suggestions...half on the machine half manually. We now realize what is involved with successfully machining both sides of the stock with the profile that we're trying to achieve...ehh it has been an aggravating process but we've learned a great deal.

Thomas it's funny you mention that because we just thought about the prospect of running some sort of convex edging router bit on the circles...but as you said, it's probably more time consuming in setup than it's worth.

Thanks again everyone,

-Pat

[twelchPTM]

I have done some "flip" parts, I really don't produce a large quantity of anything so I have the luxury of being able to use the bot to precut my blanks instead of needing to use a saw ahead of time. I create a vector the exact same size as my material in the same partfile my part are coming from but save the toolpath for the blank to its own cut file. I cut the blank, reposition it on the table and clamp runners to the edge of my table, when I flip the board I simply but it back up against those runners and everything comes out dandy.

[myxpykalix]

just thinking off the top of my head but why couldn't you elevate your part slightly off the table, cut your hole, then use a bit like this:
http://www.magnate.net/index.cfm?event=showProductGroup&theID=141
Bull Nose (Half Round) Carbide Tipped Router Bit, 2 Flute
to go to the center of your hole then then do a profile cut around the edges?
It might be hard to toolpath but it might do it in one or 2 passes (top and bottom)

[Brady Watson]

If the parts could be saw sliced from round stock, I would do that first. If not, cut out the circles and put them aside. Then screw down a planed piece of 1x8 lumber to the table and machine a series of V-shaped pockets a little less than the thickness of the material in depth. Then, make yourself some cam clamps. You drop the circle/puck into the crotch of the V pocket and cinch the cam clamp against the puck. It is not going anywhere.

You will use the vectors in software to program the machining. It should take no longer than 30 seconds to to a row of 10 pieces. Loosen the clamps, flip them over and run them again. It is safe, fast and it works. I did about 7,500 pieces just like this. It was the only way to maintain Z consistency (even .005" or so will mess up the roundover) - I got to keep all my fingers, and the quality was perfect. I programmed the tool to get out of my way after a run...It goes pretty quickly.

There's always more than one way to skin a cat...

-B

[SterlingDevelop]

Brady,

I think you are talking about putting a radius on a round "wheel".

The OPs photos look like he's trying to put the radius on the negative or "hole". Both sides.

Am I incorrect?

If the goal is the latter, the recommendations about the roundover bit in the hand held router as a second operation are very good. The router base indexes on the top of the material, eliminating the "Z" error that is possible because the CNC is indexing from the rails / carriage and because your material is almost never very flat - in relative terms.

As has been mentioned, the efficiency of the production run and the associated jigging / setup is a balancing act. If you have to make twenty of something, your setup may be diffferent from a run of several hundred.

Sometimes the faster and better way is not the CNC. But sometimes I do it with the CNC anyway, 'cause its just so freakin' cool!;)

Brent
http://www.dcscnc.com

[Brady Watson]

Brent - You are correct. Not sure how I missed that one...

-B

[backyard_cnc]

Most importantly your machine must be virtually perfectly in square in XY or you will never perfectly align a flip. Any out of square will basically double when you flip the piece over and no jig fixture or change of origin point or mirror image is gonna fix that. Check. Your machine for square first before getting frustrated with all the other stuff, been there done that and got the t-shirt

Gerald

[bobmoore]

The most accurate way to flip mirror image is to use your router to machine 4 holes near each corner of the sheet into the spoilboard about 3/8 inch. Cut the first side of the material, flip the material per your mirror image program, line up the sheet over the 4 holes in the spoilboard and tap in 1/4 inch pins through the sheet and into the spoilboard (we used the broken shank from dull 1/4 inch bits). Make sure there is no play in the pins, if necessary fill the spoilboard holes with epoxy and remachine them if they get sloppy at all. You should have perfect line up every time if you follow this procedure regardless of corners not square on your material.
Bob

[Brady Watson]

Most importantly your machine must be virtually perfectly in square in XY or you will never perfectly align a flip. Any out of square will basically double when you flip the piece over and no jig fixture or change of origin point or mirror image is gonna fix that. Check. Your machine for square first before getting frustrated with all the other stuff, been there done that and got the t-shirt

Gerald

Excellent point.

Since you already have all these holes in the board, why not machine yourself 4 precise circles that fit into the holes in each corner of the board? Just pocket them into your spoilboard maybe .060" deep or so to register them with the rest of your CAD file, and use them to perfectly align the sheet on the flip? You could tag a screw in the center of each one to keep them in place when machining the 2nd side.

-B

[jim_vv]

Greetings,

I know that this issue has been resolved, but I thought that this may be helpful. . . I have been doing more and more 3D two sided machining lately. A friend of mine sent me a helpful link (http://studiointhesky.blogspot.com/2012/04/cnc-router-setup.html) for flipping the part and indexing it on two 1/4" dowels in a fixture on the center line of the part. I just used wood dowels and screws to hold the parts in place.

I have attached a few of images of a contoured table leg that I was commissioned to cut from reclaimed Poplar barn beams which made a flip op necessary.

Kind regards,

JIM

[David Iannone]

I just cut a 2" Thick Signfoam sign double sided for another sign shop here locally. He painted the base color and paint masked. I cut the border and some lettering, then drilled 4 holes in the outsied of the peice I created just for the holes. Cut the signshape put.Flipped it, inserted 1/4" Dowels and it aligned perfect. Cut the second side. The customer picked the sign up and pulled some paint mask off, painted the second color, than paint masked it AGAIN. Brought it back to me and I machined both sideds for the finish paths and lettering. This was the first time I had EVER done 2 sided cutting, but it worked perfeclty. I also warned the customer this was my first 2 sided carve and the 2" Thick Signfoam was on him if it didnt work. I was not crazy about taking off the table and him brining it back to me after he put a second color one it. I also used a registration hole of 1,1 off of zero, just in case my home postion somehow got lost along the way. No problems, but it was a nailbiter.

[myxpykalix]

Jim,
Nice work on the table. I see you have an indexer also. Have you made anything you can share in pictures? good job:D