Concentricity Between Tool Changes

[McBuster]

Here is a toughy ... For me ...

I have a definite need to bore a grid of 10x10 half inch holes in 3/8" Baltic Birch ply. 100 total.

Here are the facts, nothing but the facts ...

- Use lower left corner as 0,0
- Always use Tch Plate for Z0

- Three Toolpaths
... - Bore 5/16" holr
... - Bore 1/2" hole
... - Use 60 degree bit for small chamfer to 9/16"

- Am very careful when changing bits. PrecisionBits Chuck & Collet

- After several attempts, always, the chamfer is not dead center. Always about a 64th+ off, which one can readily see.
- I check the concentricity by placing the 1/2" bit in the hole and looking at the chamfer
- All the holes are off the same. Down and to the right.
- Using the billet clamp Sam sells for the router

- Compared all three Scripts. Identical
- Plate is held in a fixture, all four sides and held down with two 14" bolts per side.
- I check the 0,0 before using the V Bit. Always as good as it was when starting the procedure.
- The Chamfer has been tried with a Profile and just Drilling - No difference

Thoughts? Any one? I, am stumped ...

Jon ...
Woodbury Mn

[howie0]

Just something to check. Look at your offsets. I had inadvertantly added an offset when setting up the programming in the toolpath section one day. I was pulling my hair out for a while.

[McBuster]

By Offset, if you mean the Material Setup, Use Offset X Y, they are Unchecked and 0,0. Or, in the Job setup, XY Datum Position? Unchecked, 0,0.

+++

Here is what I tried.

Made a new sample. The first three Chamfers were off. So I guessed, about -15 to the X, and +20 to the Y. Reset the X0 Y0. Chamfered 3 more holes. Better. After two more adjustments, I ended up at -6 and 13. A reduction of X one half, and one fourth. Y one half, on third. Finished all the rest. Looking alot better.

I enclose an image of the setup. By using the bolts, and placing the ply belly down, it flattens it out really well. There is a piece of ply (spacer) and 1/8" Masonite (sacrifice brd) under the 3/8" ply. Where all this sets, has been milled to be parallel of the route plane. This has worked out quite well.

Jon ...
Woodbury Mn

[McBuster]

Also, at the beginning of the run, the plate is 8.25" sqr. I made a dimple from the 60 degree bit at 4.125,4.125. After the two boring operations, replaced the 60 degree bit, went to 4.125,4.125 and spot on. Did the chamfers, still spot on.

I have no clue where else to go to see why, the chamfer op uses a different center than the drilling ops.

Jon ...
Woodbury Mn

[tag0110]

I had a similar issue and found my router was not level with the table. The easiest way to check this, is to put the biggest end mill that you have in your router. Then lower the router down to the table with a feeler gauge between one of the flutes on the bit and the table. Now check it with the other flute without moving the bit. If the gap is different, you will have to shim your router until its level. Mine was off .015 with a 3/4 end mill in. I would guess that your bit you use to drill your holes is longer than your v bit, and if your coming down to the same point at an angle. You will be off your original point.

[4DThinker]

What bit and toolpath are you using to drill out the holes? Your problem could be the chamfer toolpath, or the holes that are being cut wrong. With the flex in the Shark design, I've notice aggressive cuts can cause the bit to "pull" the router out of line ending up with what looks perfect but is actually shifted by the flex in the gantry. The fix? Slow way down. Try a conventional rather than a climb cut, or vice-versa. Take smaller steps. Use a new/sharper bit.

Good luck. I know this can be an aggravating problem.

[norseman]

I think Tag0110 may be onto something: I would not use an end mill though, I would use a dial indicator in the collet and figure out which way is out which would give you both X and Y. You can easily shim the router clamp front/back/left/right as needed.

Could also be as 4D thinker said and maybe the gantry is pulling when it hits the material, though it doesn't seem like it would be quite this extreme if this were the case.

So the question remains: is the router perpendicular to the table?

Stan -

[McBuster]

All good thoughts.

Yes, the router is perpendicular to the work, and the plane of the work is coplanar with the router.

I will slow the whole thing down and try it as a snail's pace.

I also did a test with the Scripts. Using the 60 degree bit, I ran to .500" Script but only put a dimple 1/32" deep with the 60 degree bit. Then, did the same for the Chamfer Script.

Spot on. Dead Center. There is nothing wrong with the mechanics nor logic.

Will run down and try The Slow Version.

Problem is, if this -is- the case, being too aggressive, each unit I produce takes two plates. If, it will take a half hour per plate, that is only eight sets a day. That, is not enough.

Jon ...
Woodbury Mn

[rungemach]

Hello Jon

It already looks like you are doing a roughing and finishing pass type routine, which also requires bit changes and re zero operations along the way.
all of that can be time consuming if you have a particular job that will be run repeatedly.

Something that has been said before in the forum here, and also over at Vectric's forums, is that the feed rate can be an issue with these lighter (non-comercial) machines. The values that come default in Vectric software may lead folks to believe that they apply to the Shark, when in fact they are aggressive feed rates for that class of machine. It is easy to feel that if a machine can do 200 ipm rapids that it was designed to cut at that speed with full accuracy. If you are doing "production" on a machine, the temptation is always to explore how quickly the job can be done.

Commercial class machines are made to be able to use the router bits at their optimum cutting and wear speeds, which require very sturdy machines.
So compromises have to be made with the lighter machines.

You do not say what IPM you are using for your project, so it is hard to judge whether it is too fast. If the quality fine at say 10 ipm, and gets progressively worse as you go up, you know it is a speed related issue and can work to find the best compromise point. You may also have z axis freeplay or flex which shows up in hard plunging operations like aggressive drilling.

You may need to look into fixturing that job " multi up " to get good productivity out of your machine. You could mount 4 parts in a single fixture and do each operation to all 4 as if they were one larger part if you can get to a speeds and feeds point that gives you the quality you need.

If you haven't done this already, I would also go over every bolt on the machine to be sure they are all tight and there is no free play anywhere.
Also, check if you have adjustable bearings on your x and y linear rods, and if so,that they do not have free play and also run freely. If you are having a "lost steps issue" it should show up in a failure to return to the same physical zero point after a cut is done although your controller will say (and think) it is at zero.

[McBuster]

I am embarrassed, but i have a problem in the Rate of Feed.

I did some tests at 5 10 15 20 and 25 ipm, and the lower speeds are looking much better. I will reduce the feed rate.

With thinner plywoods, I may not be able to reliably do a 2-up, 4-up or 6-up. My goal right now is to dial in all the variables so I can repeatedly make units that look and work great.

Thanks for the time taken to help me out.

Jon ...
Woodbury Mn