Hold down/fixture/cutting help

[eklug]

I think i might need a better way of holding down these blocks. These are rv fascia corner blocks and they get a square shaped inlay into the top of the block. It is just a very simple 3" square with .25 radiused corners. The shopbot cuts the inlays out of .25" laminated material and also cuts the pocket out of the blocks. You'd think it would be a good match. Never. The pocket is either too small or too large. I keep changing the program size (in partwizard). Right now it is programed to cut 3.04" square and the machined pocket comes out around 2.98-3.01". It is a little off-square. One side is usually up to .02" smaller than the other. The straights of the square also seem to be slightly curved. What could be causing this?
Do I need a better hold down method? I dont see the parts moving at all. Right now there is a fixture screwed into the table and clamps that hold the part into the fixture.

Please help me get this working right. I just dont know what to do with it anymore besides just giving up my desk job and doing it myself. Sigh.

5019

5020

5021

5022

[Brady Watson]

Emily,
Just off the cuff, I'm seeing steps in the area clear section of the left jig. This tells me that you Z axis *may* be out of perpendicular with the spoilboard. When you surface the spoilboard, how deep are the ridges?

Secondly, how fast and how deep are you cutting? Just as a reference, I would keep what you are doing and run the toolpath very slowly. Just try running it at let's say 1.2 IPS using a .125" stepdown. Check the dimensions of the part after doing this. The slower speed and stepdown should keep the material from moving and give you a very accurate part.

-B

[paco]

That look like a very well rigged JIG.

I second Brady's idea and if it solve the issue you could optimize the toolpath(s) for a quick rough than a finishing profiling pass so you get both of the best; fast and accurate.

[ed_lang]

I like those clamps!

Who makes them.

No don't tell me! That will be something else to get and test out.

[eklug]

Off hand I don't remember how deep those ridges were when i surfaced the table. Its been a few months and it needs surfacing again. Is there a surefire test to tell if the z is perpendicular? How can it be fixed?

The parts are usually run about .25" deep @ 3ips. Running it slower than that really chews up the vinyl that these parts are wrapped in. A faster cut like 5 ips leaves a smoother cut. I think multiple toolpaths would confuse the operators too much.

[paco]

Toolpaths can be assembled into a main one. What I have in mind is a "rough" 2D area clearance (pocket) with, say, a 0.05 to 0.15" allowance then a profiling pass at the final pocket depth is ran slowly (enough) with no allowance to the final intended size. Once you got both toolpath running the way you want and reach the spec. size, you get them together in a main file that call each one. Still just try what Brady suggest before going any deep into toolpath programming other than you already did.

I don't understand the vinyl chewing thing... sorry...

[zeykr]

I'm interested in what part the tennis shoe plays in the operation.

[harryball]

Let me ramble, see if you can find something to use...

I curious why you didn't try a vaccum holddown with a puck. While this jig and clamp method looks solid, I'm wondering if you are not seeing the same thing I was getting with a project I was doing. I was clamping the board with cam style clamps and tried several different jigs with tremendous pressure. Yet, every time the pocket overlap I was cutting always had some gap or out of square to it. My solution was a vac puck with 23" of vac behind it. My first attempt was so tight it looked more like an inlay than a lap joint.

I also had an issue with my table top moving on a project. The bleeder board was screwed to the table top on the corners and one in the mid section each side. I was having problems with a project I was screwing to the table top and running. The cuts were not accurate by a small amount. I discovered that by running the vac holddowns even though the part was screwed down the problem went away. The bleeder board was moving ever so much without vac behind it. Glue fixed that.

Bit and/or gantry deflection. This one got me recently. Without something behind the bit while cutting it can deflect. This deflection is minute but present. I solved the problem by making a very fine clean up pass after doing my pocket and running it slower than during pocketing.

For squaring Z I've adopted a perhaps strange but effective method. I use the spindle wrench with a bolt in it and the Zzero plate. I hang the wrench on the spindle and zero the Z out on the end of the wrench. I then use the keyboard moving at fixed intervals of .01". Then I move the Z axis up until one click makes the connection go off. Then I turn the wrench 90 degrees and compare with the zzero plate. I try to shift 1/2 of the gap out and then repeat moving the Z axis .01 each time.

My goal is to get all 4 quadrants of the wrench so the contact comes on within +- .01" I'm currently squared 8" out from the center of the spindle as follows

Y+ 0.01

X+ 0.01 0.02 X-

Y- -0.01

This may not make much sense unless you see it but it doesn't take too long once you get the hang of it and doesn't require any special tools. Just a small bolt screwed into the hole in the end of the wrench.

Robert

[benchmark]

Hi Emily

I use a combination of air ram and vacuum hold down for machining our wood boxes, the red tubes on the right of the jig are the vacuum tube. This works very well for machining 20mm deep.

Another thought would be to align the blocks so the pocket is aligned in the X/Y direction this would help with the accuracy, the Shopbot will not be cutting a diagonal path.



Paul

5023

[mrdovey]

Emily...

I assume you're cutting these blocks with a 1/4" bit - please correct me if I'm guessing wrong.

I'm also guessing that you're "climb cutting" the pockets.

You might try running the pocket program twice on the same block (without unclamping the block) and seeing if the result is closer to what you wanted and posting the result.

...Morris

[fleinbach]

Emily,

Brady's suggestion is the same one I gave you in your other post questioning this. Too deep a cut or to fast will cause your problem. But since you said your cut quality suffers there is another solution. With this solution you can keep your speeds the same. First you need to cut about .03 undersize then make a cleaning path for the final cut. This has always worked for me in maintaining size acuracy.