Deflection

[mx_urfer]

Hello, I am using a prs alpha machine to cut cabinet parts for our business. We have experienced some technical difficulty in that our parts are all coming out 1/8 too short and narrow. this is proving to be a problem. it is not the cabinet software we are using to design the cabinets. I first thought that it might have been a unit values problem but they were in fact set correctly. I called the shopbot tech support line and they claim that it is deflection of the bit or the z axis. I don't believe this is caused by the bit because it would snap if it were to bend even a small amount. If anyone has any comments or suggestions it would be greatly appreciated.

[ed_lang]

If I may suggest a couple of things to "test".

Install a V bit or use the edge of the cutters you have and move the machine from say 0,0 to 95,0 and measure the amount of travel the machine moved. If it moved 95", then the unit values are right and the machine is moving like it should.

Next verify the size in the CAD drawing you are using. Then verify the diameter of the bit you are using. Don't get fooled by thinking all 1/4" bits are in fact 0.2500".... They are NOT. Measure it and put that value into the tool database. Then cut the part and measure it. If you still find you are off, then I would install a 3/8" or 1/2" cutter, but sure to measure it! Then re-tool-path the part for the larger cutter. Cut the part and measure.

I have a feeling by doing the above steps you will discover you source of wrong size parts.

Let us all know how it goes.

[seana]

Max,
Are your parts small in all directions?

First check the size of your bit, mic it don't presume thats really .25
Then check the settings in your tool path program make sure the bit you picked for tool pathing is the same size as the one you just measured.
Also make sure that in the tool path program that you don't have an offset checked by accident.

I typical cut (regardless spindle or router) in two passes when i use a .25 bit. First with an offset of .o4 to a depth of .6 (in .75 material) then i do a final pass on profile and to full depth. It produces a nice edge finish and the parts are on spec and i don't have to worry about any bit deflection.

You would be surprised on how much bit deflection you get without the bit snapping.

Hope this helps you narrow down your search.

Sean

[beacon14]

Not just cutter deflection but any looseness or slop in the machine's assembly and adjustments can contribute to your problem. Double check all bolts for tightness and all rollers for proper adjustment, especially the Z axis rollers.

[myxpykalix]

Maybe this has been said but if your part is being cut at a consistent 1/8" difference in all places then bit deflection would seem less likely to me than the toolpath operation. Depending on whether you are cutting inside/on/outside your vectors would give you a uniform difference all along the pattern.

Do you have the ability to draw the cut pattern onto the part first? As an example i was unsure about a cut in a customers wood so the pattern was drawn on then i put a point laser beam in the router and ran the file and it followed my lines. I knew i was ok to cut. Your situation may not be applicable but this might give you some insight to whats happening while there is no cutter load on the router.
Bit deflection seems like it would not be a consistent size all around due to the cut pattern (short lengths vs longer ones) but i am NO expert, just my 2pennies worth.

[knight_toolworks]

tropical hardwoods seem to deflect bits about the worst but even there with cutting 1.5" deep with a 1/3" bit I never got 1/8" deflection. so I doubt thats what the problem is.

[kirkkelsey]

Max,

In addition to Sean's great advice, I wanted to chime in about a similar lack of accuracy problem in cutting to the line when Sean was cutting the Blind Dado joinery for some cabinets where I provided the DXF files. It was not until he replaced his router that we concluded some of the deviation was from run out of worn bearings.

Here is a history of our efforts to manufacture Blind Dado joinery for cabinetry.

1. Input actual mic'd value of bit diameter (we use actual 0.246" value for 1/4" bit). He codes in VCarvePro and I in MasterCAM.

2. Removed play from machine. Vibration from use probably loosened some connections (which Sean found through persistence).

3. Removed run out with new router/bearings.

4. Changed finish pass from 0.015" to 0.030" or 0.040" because there was not enough "bite" that the bit deflected so that the pocket measurement was the same as before the finish pass (conventional cut).

5. Varied cutting direction between climb and conventional cut. We are trying to match the face created by a 3/8" deep pocket cut to create the blind tongues, and the 2 pass Profile/Contour cut as listed by Sean above. On the X0 end of the Top and Bottom parts, we had to use a climb cut, and the X96 end a conventional cut to get both cuts to line up with a smooth surface between the 3/8" deep pocket and the through profile cut. We are cutting tough and fibrous Bamboo Plywood. Bit deflection varies significantly between cutting cross grain and with the grain (surface skins are about 1/8" thick with single solid core rotated 90 degress).

6. While we still have a 0.019" variation in surfaces on an X96 face of 2 parts, we have compensated by shifting the toolpath on the left side of the pocket an additional 0.019" from the pocket outline defined by the DXF file. Until we determine the proper setup to remove this bit deflection, it provides the smooth surface we require.

Sean Aydlott is cutting out cabinetry with Blind Dado joinery for both the Ends and Back. We have been able to eliminate all screws through the cabinet ends, and instead substitute a brad nail through the end grain of the ends to pin the tongues in place until the glue dries. Screws are still being used to pull a 3/4" back into a 3/16" long tongue milled on the back side of the Cabinet Top and Bottom.

[daski]

we have found that with a 1/4" bit we get .017 bit deflection. We just adjust the bit diameter in the tool setup.

[gpari]

For those that adjust the tool diameter or account for bit deflection with a toolpath offset, how to you deal with the change in deflection caused by ramp speeds. As the tool slows down to change corners, the cutting forces go down, and so does the associated deflection. You're still not cutting a straight line (I guess if you are cutting circles, where the feed rate never changes, and using lead-in/outs it would be fine).

The easiest way I have found to deal with deflection (which can be as much as .040" on my machine at 9 ips & .625" into 18mm baltic birch) is to run 2 passes. First pass is about 75-80% of material depth and run in the CLIMB cut direction. Second pass is into the spoiler and run in the CONVENTIONAL direction. This eliminates any guess work for offsets or trying to fool the machine about what size bit you have. And as the bit dulls and cutting forces go up causing the deflection to increase, you still end up with parts that measure net.

I know this won't fix the original posters problems, I agree he has a software, mechanical or setup problem. Just sitting in the field enjoying the view when this train jumped the track and came right at me


Gabe

[mx_urfer]

Thank you, I have done some experiments with a v bit and I have tried a number of different types of bits cutting a small part many times trying different feed rates and spindle rpm.

So far the best results as far as coming closer to an accurate measurement and clean cut, have come from a 1/4 inch single flute carbide tipped bit with a CEL of no more then 7/8 to keep the choke from hitting the material.

As far as feed rates I have had good time results and less deflection running at 4 ips at between 20 and 24,000 rpm. These changes have gotten my machining accuracy down to less then 1/32 of right on the money.

Max.