Bit deflection-how much is to be expected

[mike_annetts]

Hello

I teach at a small school and we are using the bot for mainly cabinetmaking. we are running into a problem of our dadoes and groves not being the correct size. the bot is not cutting .75 grooves at the correct size but instead they range from .725-.76.

I have done the following

checked the table squareness

all bearings tight and the table rools smoothly

router moves accurate distances in the x and y axis

new bearings in pc router

all set screws tight

bit diamater verified



I have cut 3/4 wide test grooves in "strawboard" (similiar to a soft particle board)all to a depth of 3/8 of an inch. some in 3 passes and some in one pass. this material is quite soft so I didn't think that bit deflection would be a problem. All cuts were done at a a feed rate of 1.25 inches per second at 16000 rpm. It seems that in order to be fairly accurate I have to do climb cuts in 3 passes. one pass at climb cut would be .725 - .735 inches wide while one depth pass with conventinal milling would result in .763 - .76.
Taking 3 1/8 deep cuts with conventional milling resulted in cuts from .759 - 757. Again all grooves were .75 inches wide using a 3/8 straight bit (2 flute). I tried the cuts with bothe the control software and Mastercam whic posts diectly int0 shopbot code.

My question are these reasonable figures for the bot. i can see some diference in climb vrs conventional but this is pretty soft stuff and .35 is not tht deep with this material ANY feedback would be apreciated.


Thanks
Mike Annettts

[richards]

When I cut sheet material using a 1/4-inch or 3/8-inch bit, I cut most outside profiles 0.020 - 0.040 larger than desired and most inside profiles smaller by the same amount on the first pass. On the final pass I cut to the desired dimension. Also, I nest parts with a spacing that equals the bit diameter plus 0.080 inch to allow for a rough pass and a final clean-up pass on all edges.

When cutting dadoes, I make one pass down the middle of the dado, using a bit with a diameter at least 0.080 inch smaller than the width of the dado, and then a clean-up pass on each side of the dado to get to the desired width. With the Alpha and a Porter-Cable router, speeds are 4-8 ips on the initial pass and 10-12 ips on the clean-up passes. Jog speeds are 30-ips on the X-axis and the Y-axis and 6-ips on the Z-axis.

When I cut lumber, I usually make the initial pass with a climb cut to reduce splitting and tear-out, with the subsequent passes being conventional.

Like you, I spent quite a bit of time trying to adjust the sloppiness out of the machine; however, one day, when the full sheet of MDF that I was just beginning to cut, a sheet that weighs about 80-90 lbs, lost vacuum and was pushed more than 12 inches by a little 1/4-inch bit, I realized how much force was being exerted on that little bit. After that, I stopped fighting bit deflection and started making multiple passes.

Mike

[mikejohn]

According to the specs for the PRAlpha, the overall cutting accuracy is given as 0.015".
Does this mean that Mike should expect his .75" grooves to be anything within .735" to .765", with his machine working perfectly within spec?
Or does overall cutting accuracy mean something else?
Positional accuracy is given as 0.005". I am unclear as to the difference between the two. To get the true accuracy, do I need to add these two together (0.02")?
If this is how it works, then Mike can not expect better than .73" to .77" (which is what he is experiencing).
This accuracy of .02" equates to 0.5mm, the accuracies other shopbotters have suggested is what I am likely to achieve.
Or am I once again missing the point?
....Mike

[mikejohn]

3846

[elcruisr]

I'm with Mike Richards, you will get alot of bit deflection with a 1/4" tool. I follow the same tactics when using smaller diameter tooling, rough pass and finish pass. If possible try the same tests with a 1/2" tool and test your results then. We have found for many of our applications that a 3/8" tool is a good compromise between stiffness and cost.

As to accuracy, we usually can beat the .015 overall cutting accuracy by keeping the machine well adjusted and using sharp tooling (dull toolng causes a large increase in cutting force and more deflection) and roughing, finish pass tactics. Usually around .008 or so.

Eric

[fleinbach]

I have made several posts pertaining to this issue in the past few months. Once you understand just how much cutting forces are exerted on the tool when cutting at varying speeds and depths it will be eaisy to obtain the acuracy you require.

To get the acuracy using the Shopbot several factors need to be considered. The first thing is make sure all parts are tight and adjusted to there closest tolerances. Particularly the roller bearings on the Y car, they are the most important at keeping the bit on track. Adding a second Y motor would greatly reduce this deflection, but this is realy not nessacary if you are careful with how you make your cuts.

How large a bite you take at one time is most responsible for the bit wondering off track. Speed of cut is less of an issue but does affect descrepancies. It seems that if you minimize depth of cut by .25 or less the force exertied will minimize error between .005 and .015 depending on the material being cut. Once you cut 3/4 material in a single pass the forces are enormus as are the descrepancies. I don't have vacuum yet and using only 2 screws to hold down a 1" sheet of MDF, making a single pass cut, I have seen the 1/4" up spiral bit lift the MDF completly off the table. That sheet weighted 130 lbs.

Mike Richards has given you one method to optain acurate cuts.

[Brady Watson]

Lots of god advice in this thread. I'll jump in here and say that you should use the largest bit you can for the job. There is a HUGE difference in cut quality and accuracy when you step up to a 1/2" tool.

I recently did a job where my dadoes had to be exactly .68" wide and .375 deep in mahogany. I used a 1/2" bit, 2 passes at 12000 and 2 IPS. The material was held down with vacuum. The cuts were absolutely dead on and verified with a digital caliper.

If your cutting an inside profile, use Climb. Outside, use Conventional. If you must use a 1/4" bit, then slow your speeds down if you are losing accuracy.

-Brady

[richards]

As the others have mentioned, a 1/2-inch cutter is much better than a 1/4-inch cutter when deflection is a problem and the 3/8-inch cutter is the best compromise between overloading a Porter-Cable router and maximum efficiency.

I always reach for a 3/8-inch cutter first unless something about the design or nesting requires a 1/4-inch cutter. Because of the Porter-Cable router that I'm using (and my work methods), the 1/2-inch cutter is always my third choice. It gives a much cleaner cut, but it requires fairly shallow passes.

Perhaps my procedure is faulty, but I always start by checking the desired chip-load with the chip-load calculator (available for downloading here in the forum). Knowing that the best speeds on the Porter-Cable 7518 are 19,000, 21,000 and 16,000, in that order (best speeds for me as a compromise between power and noise), and having an Alpha with a large range of possible feed speeds, I select the desired router RPM, use the calculator to get the desired feed speed and then make a few test cuts to see how deep I can go before the router starts to bog down. Using those steps, I know that I'm making the biggest possible cut to hog out as much material as possible per cut. Then I make a high-speed clean-up pass to even-up the cut.

A side note to Mike John about accuracy. The Shopbot is "repeatable" within my ability to measure from any point on the table to any other point on the table WHEN I'm just measuring positional accuracy. However, when I'm cutting, the bit always wants to take the path of least resistance through the material leading to errors caused by deflection In my mind, the deflection has nothing to do with the accuracy of the Shopbot and everything to do with the material being cut, the cutter making the cut, and the perameters of the program used to make the cut. Knowing "what" is causing the error allows one to "work around" the error, hence my use of creating a rough pass and a final pass. Being very limited by the Porter-Cable 7518's lack of power when I try to make aggressive cuts with a 3/8-inch or 1/2-inch cutter, I'm sometines forced to compromise and use a 1/4-inch cutter and then program in multiple passes. (Please note that stating that the Porter-Cable 7518 is underpowered is not a slam against Porter-Cable, although I do believe that their hands should be slapped for rating the router at 3-1/4 hp. It is simply a statement of fact. At some point, a CNC router operator has to realize that getting the full potential out of his machine will require a heavy duty, powerful spindle instead of a relatively light duty router.)

Mike

[mike_annetts]

Hello and Thank you for all of the replies. Mike Richards (a lot of Mikes here, I like your idea of running the bit down the center of the dado or groove and then making two passes to finish off the width. I have enough trouble getting the students to figure out the dadoes now without cutting then undersize and then making finish passes so I think that I will pass on that idea. These students are completely new to this stuff so I have to keep it very simple. Good tip though. Shopbot suggested the collet may be out but I tried another with about the exactly the same results so I can rule that out. I will try Mike Richards idea and see what happens. This forum is extremely helpful as always.

[mikejohn]

I endorse the value of what you learn here.
This thread, along with many others, seems to say one important thing.
Give the shopbot the opportunity and it will cut as accurate as you want.
But choice of bit,rpm,machine movement speed, depth of cut,climbing, and method of arriving at final tool path all need to be right.
To put it another way, do it 'wrong', which normally means trying to complete the job in the short a time as possible, may give you a much poorer result as getting all the above right.
I sincerely hope this is true, each day I get closer to owning my shopbot. Just awaiting freight details to UK at this time!
.......Mike

[pcathome@telesal.net]

I cut 5/8" double sided melamine with 1/2" bit in one pass , and normally I get accurate results. Now I changed to 1/4" bits with 1/4 shank in order to double my speed and I'm getting about 1/2 a milimiter off even without doubling the speed
. Has anybody tried 1/4" bits with 1/2" shank ?
or 5/16" with 1/2" shank ? I woould think the 1/2" shank should minimize deflection ????

[Brady Watson]

Alberto,
A 1/4" tool deflects quite a bit in 5/8" material running it at full depth. It is often false economy to use a 1/4" bit and 2 passes to save 1/4" of material/kerf. Depending on the material, you may not be able to live with the 'waterline' marks that a 2-pass/ 1/4" setup gives you...but you could cut it in 2 passes over size, and then go back and do a cleanup pass to get rid of the waterline marks. Again...false economy. I have found that a 3/8" bit is a happy medium between the 1/4" and 1/2", although there are less choices in bits that size. The length of the bit can also influence deflection. IE- a .75" LOC bit would have less deflaection than a 1" LOC one (LOC = Length Of Cut)

The general rule of thumb when choosing a bit for your material is, don't exceed 1.5X the cutter diameter per pass, or in the case of a 1/4" bit, no more than 3/8". Using that rule, a 3/8 or 1/2" bit is the right tool for cutting 5/8" material in one pass. You also want to learn to get a feel for chipload. You want the biggest chip (to pull heat away and minimize the tool rubbing...and creating more heat) while leaving the nicest edge. Watch what kind of chip comes off of the bit. You NEVER want to be creating dust when you cut parts. Only chips. When I cut new material, I set a baseline and start observing and asking myself thee questions:

-Does it LOOK right? How big are the chips? Edge Quality? Is it on spec?
-Does it SOUND right? Is the router bogging? Excessive vibration?
-Does it SMELL right? Am I burning? (MS too low or RPM too high...not disco inferno)
-Does it FEEL right? Are the edges jagged?

My feeling is, when you are cutting clean and on-spec parts, write down what speeds & bit you ran and keep a log...then you can solidly rely on your previous jobs to gauge new ones.

Hope that helps,
-Brady

[dvanr]

Alberto,

Is the cut your making the same width as the bit diameter?

1/4 to 1/2 reducers sometimes introduce runout side to side. Making the bit cut wider than its actual measured width.

[oddcoach]

i use an onsrud 60-111 bit to cut 3/4 inch material in one pass with very good results. feed speed around 2.25 in per sec. the tec guy from onsrud gave me this recomendation. i was cutting in 2 passes before but had breakage problems. since i went to 1 pass i have not broken a bit in over a year.
john

[elcruisr]

John,
We've been running 60-111 tools in 3/4 ply and 3/4 melamine and have found you can push your feed rate up to 4.5 to 5 inches a second at 16,000 to 18,000 rpm. get about 8 hours production out of a tool before resharpening. The 60-121 (3/8 dia) is still our most used tool. It can run all day in 3/4 stock at 10 inches per second.

I would agree with Brady that a 1/4" tool is often false economy. We only use them due to part constraints (Like all the 1/4" vent slots we have to cut for one customer) or small pocketing or boring. I wonder about Alberto thinking he can double his speed with a 1/4" tool or did I misunderstand him? To go faster you need more diameter to prevent breakage. The big boy rockets pushing 50 inches a second are running 3/4" tooling!

[gerald_d]

Alberto's problem is maybe hauling away the sawdust? A 1/4" bit makes half the dust of a 1/2" bit.

[mikejohn]

If you have a 1/4" bit and a 1/2" bit rotating at the same R.P.M., moving forward at the same number of inches per second, then the 1/2" bit removes twice the material per second as does the 1/4" bit. As this material is being removed by the tip in both cases, then the load on the 1/2" bit must be twice that of the 1/4" bit. If your shank size is 1/4" in both cases, isn't the breaking point at the same load for both?
To achieve the similar loads for each bit you would need to move the 1/4" bit at double the inches per second to that of the 1/2 inch bit.
Therefore,it also seems to me that to achieve an ideal chip size, either the 1/4" bit must rotate at half the speed of the 1/2" or it must move at double the inches per second.

.............Mike

[Brady Watson]

Mike,
A 1/2" Diameter tool has 4X the surface area and volume of a 1/4" tool...So no, it is not a 2:1 ratio when comparing identical carbide material bits by diameter alone.

I would say that yes you are correct in saying that a 1/4" bit must travel twice as fast as a 1/2" bit to remove the same material in the same amount of time...but that doesn't take into consideration that a 1/4" tool is 4 times more prone to flex than a 1/2" tool under the same chipload.

If you are going to run 1/2" diameter tools...use a 1/2" shank! (Just re-read your post mike...yes you are correct...) What's the point in running a 1/2" diameter tool with a 1/4" shank other than 'It came with the cheap set I bought when I 1st got my bot' ? (I still have some of them!)

-Brady

[gerald_d]

If your router is under-powered for a 1/2" bit, that same router might be able to push a 1/4" bit at twice the speed?

(There appear to be some factual errors in the maths above, but I don't want to spoil your fun...
)

[mikejohn]

Brady
The volume of a 1/4" cylinder (Pi*r*r*height) is 4x that of a 1/2".
The surface area (Pi*d*h)+(2*(Pi*r*r)) will vary with the height of the cylinder, but will be less than 2,5 times, unless the cylinder height is shorter than the diameter of the cylinder.
However, neither the top of the cylinder (tool) nor the bottom come into play, so the surface area we are interested in is 2x for the 1/2" over the 1/4"

Are you suggesting that you need a collet to fit all sizes of bit, so that the shank is of an equal diameter to the cutting edge?
.............Mike
edited to say Geralds post crossed with mine

[gerald_d]

May I suggest that you don't get confused volumes and surface areas of cylinders? The important issue is the kerf width and the volume of material cut out.

[Brady Watson]

Let's not split hairs with the math...because it really doesn't matter. I think that we all have the formulas memorized at this point (or should). What DOES matter is edge quality in comparison to time. A 1/2" tool, depending on detail of profile, puts a nicer edge on just about every material I have experiemented with.

In a way, yes Mike I AM suggesting that you use the right tool for the job. If you are running a non-spindle tool, then your choice in collet size is limited. However, if you are running a spindle, then you have no excuse not to use the right tool for the job. You don't process panels with a 1/4" shank, 1/2" diameter tool. If using 1/4", then use a 1/4" collet. The spring collets that are used in spindles can expand and contract a small degree to accomodate just about any diameter bit that is appropiate for use on that tool.

If you want high-quality parts coming off of your machine, similar to those that the 'big boys' cut on their $250k machines, then don't use beat bits. If you want 2nd rate cuts, then use the cheapies for everything. Cheapies have their place with your CNC, but not on profile passes for a customer.

-Brady

[gerald_d]

Poor old Alberto must be shaking his head by now..

He is concerned about the deflection on a 1/4" bit and asked the question "Has anybody tried 1/4" bits with 1/2" shank ? or 5/16" with 1/2" shank ? I would think the 1/2" shank should minimize deflection ?". Can't we spare him the sermons and give him a straight answer?

Alberto the bit flexes inside the wood, as well as between the wood and the collet. If you put a thicker shank on your 1/4" bit, you will only reduce the flex between the collet and the wood, not inside the wood. Another way to reduce flex is to get the collet as near to the wood as possible - it won't help to thicken the shank if the stepped tool has a long shank lifting the collet higher above the wood. Consider making your cutters shorter, even by cutting off some of the length on the collet side (use a thin grinder).

[paco]

Just to add something about Brady's remarks about router collets; the Milwaukee 5625-20 have 1/4", 3/8", 1/2" collet available (Hummm... PC7518 too)... just no 1/8" (I would really like that)...

By the way, High Speed Steel flex much more that Solid Carbide tool bit...

[ron brown]

By the way - all you mathimatical whizburds, while strength is on the square of the part, stiffness is a cube factor. A 1/2" bit will be 8 times as stiff as a 1/4" bit.

Ron

[mikejohn]

Why does flex cause a wider kerf?
Is it wider at the bottom than at the top?
How does it come about?

3847
If the tool is travelling in the direction of the green arrow, then the force on the tool is as shown by the red arrows. This force is evenly spread around the tool as it rotates. I recognise that when the bit is in the position shown the cutting tip has a force exerted on it from the right, but a quarter of a turn earlier the force was in the same direction as the red arrows, a quarter of a turn later and it is opposite the red arrows.
Why does it flex?
Do you mean the tool bends like a banana?
.............Mike

[srwtlc]

Mike, add a rotation arrow to the bit in your diagram (clockwise). Now, what directon does that bit naturally want to go as it's pushed forward? That banana is going to want to peel off to the left as it's pushed along it's intendend path. Thus, with your smaller diameter bits, they deflect more, leaving not so much a wider kerf as they do a skewed kerf maybe.

(Edited) For our fellow Botters in the southern hemisphere, do your routers turn the other way? And do you have to buy left hand spiral bananas?


Scott

[mikejohn]

Scott
I see that now.
Does the flexing occur at the point the tool enters the wood, as shown in the drawing, or does it flex from the collet?

3848
Is it a 'straight' flex as in my drawing, or curved?
Or is the collet being 'flexed' to one side?

..............Confused

[gerald_d]

"Bit deflection" is not the sole source of deflection - there is also deflection in the structure of the ShopBot. Mostly (with short cutters), the gantry deflects more than the bit, particularly if the y-car is in the middle of the gantry. It could very well be that one sees less total deflection with a smaller bit, simply because the pushing forces are lower.

[mikejohn]

So there is no 'bending' of the bit at all?
This is beginning to make more and more sense.
Now it begs the question, if I am cutting through 20mm softwood with a 6mm bit, and a CL of 21mm, is the bit going to have a smaller chance of breaking if I cut full depth, with the collet nut brushing the surface of the wood, or do I do a first cut of 10mm, and a second cut of 10mm, where the cutting force stops half way along the length of the bit?
Or is this now a different problem to the forces producing flex?
...........slightly less Confused

[gerald_d]

There certainly is 'bending' of the bit - everything 'bends' (or deforms) under load. The extent of the bending may be small or big, but it is there. Other things may be bending more or less than the bit, but they are also 'bending'.

'deflection' and 'chance of breaking' are not directly related to each other. If the cutting force on the cutter is F, and the distance of the cutting force from the collet is d then
- 'chance of breaking' is F x d (doubling d will double the chance of breaking)
- 'deflection' is F x d3 (increase d by 26% and the deflection doubles)

The above assumes that the cutter wants to break at the collet. But it often breaks lower down where it is cut away to form the flutes

Scott, the Belin company makes bits for left-hand routers - wonder who actually uses them?

[normand]

Gerald carving machine can have 10 spindles on each side of the model to be copied 10 turn clockwise 10 counterclock

[mikejohn]

Gerald

You say There certainly is 'bending' of the bit - everything 'bends' (or deforms) under load.
The part I can't get my head around is this. The bit is rotating, so whatever forces are being applied, are applied to a different part of the bit, moment to moment.
So does the bit continuously change its direction of bend?
..........more Confused than ever!

[gerald_d]

Normand, that is interesting! (Will send you an e-mail soon asking your opinion on 500 identical carvings)

Oh yes, the bit is changing its direction of bend all the time - causing lots of fatigue.

[Brady Watson]

If you want to see a good example of bit deflection, chuck a 1/8" RotoZip bit in your router and cut a square in a piece of scrap wood 1/8" deep...You can see the bit 'trailing' behind the collet in every direction...If you're lucky, it will catch up at some point during the cut!

-Brady

[richards]

Gerald,

Who uses left-hand routers? That should be self-evident - left-handers! Those of us who were fortunate enough to be born left-handed appreciate companies like Belin who accomodate our left-handedness. It's still a real hassle to have to re-wind the routers to have them turn in the 'proper' direction, but us die-hards consider it to be a sacred duty to 'fix' the direction that things tend to go, if left uncorrected.

-Mike

[gerald_d]

I never could understand why 'lefties' made such an issue of the world being against them - until my wife made me cut out a dress pattern holding the scissors in my left hand. It is painful!

[normand]

Mike I understand That you can change the rotation by rearanging the wire but what about the collet ,it has to be left hand thread or the bit would get loose when you start the motor

[mikejohn]

Gerald, could you whip me up a little high front, low back number for the main social occasion at the September European event?

[bruce_clark]

Hey,

We lefties are the most discrimated group of people on Earth but we are the only people in who are in their right mind!

Here are some more example:
Lefties have suffered a long history of oppression and alienation. "Left" was generally synonymous with "evil," and in most societies left-handed children were forced to learn to write with their right hand.
Language isn't exactly sympathetic to lefties, either. Having two left feet is an insult to your dancing skills; left-handed oaths are promises you don't intend to keep; and leftovers are generally not appetizing.

The words "dexterous" and "adroit" are both derived from the Latin and French words for "right," respectively. And the Latin words for "left"? Try "sinister." Even in sign language, raising your right hand means "powerful" and "brave," but covering your right hand with your left means "death" and "burial."

No, really, left handed people live, on average, about 9 years less than right handed people, though this site disputes that claim:
http://www.drdaveanddee.com/left.html


For more, check out this site:
http://www.discardedlies.com/entries/2005/02/end_the_discrimination.php

Proud to be a lefty,
Bruce

[mikejohn]

We drive on the left

[gerald_d]

"left handed people live, on average, about 9 years less than right handed people" reminds me of the other important statistic:

Married men live longer than un-married men, but they are much more willing to die!

PS. Left-handed scissors are freely available if you ask around - there's a tip for Mother's Day (for some).

[bruce_clark]

Mike,

Y'all even vote left! I saw that Tony got another term.

Bruce

[mikejohn]

Gerald
Married men don't live longer, it just feels that way!

Bruce
Actually a little over 63% voted against Tony!
A wierd system where a little over a third of the votes gets you 60% of the seats, whilst over a quarter of the votes gets you around 10% of the seats! And ours is called the Mother of Parliaments!

...........Mike

[simon]

I would give my right arm to be ambidextrous.

[D. Burch (Unregistered Guest)]

Everybody is born right handed. The intelligent ones overcome it.

[seymour (Unregistered Guest)]

Married men usually die before thier spouses. It's self defense move.