Spoilboard surfacing tool question

[Chuck Keysor]

Very shortly I will need to surface the spoilboard of my PRTalpha 5'x12'. Roughly speaking, a new 1 1/2" diameter planing bit is around $50. Yet a couple of people on past posts have said that they like the Amana surfacing tool with replacable knives. The Amana 1 1/2" bit costs $169. And that includes a set of the 4 sided knives.

So, it looks like if someone throws away their $50 regular planing bits when they go bad, that the $169 bit with four sided blades would be cheaper. But I don't know about sharpening costs and more importantly, the quality of resharpened bits.

As added information: A friend of mine has maybe 40 rough sawn planks of heura crepitans (spelling?) that are 14 inches wide, 8 feet long and 2 inches thick. I have two, and another friend has maybe 10. Flattening these boards prior to further processing is very difficult because of their size and weight. I would like to use my ShopBot to do this type of work on occassion.

Questions:
Is it the better option to buy a conventional planing bit for $50 and just get it resharpened whenever it gets dull? Or are there problems/costs associated with sharpening conventional bits that make buying the Amana RC2250 the logical purchase?

As a guess, what would be a logical number of replacement blades to keep on hand given my intended application?

Thank you, Chuck

[bleeth]

Replacement blades are cheap. Buy em by 10 or so.
Re-sharpening a surfacing type of bit should be no issue if your local grinder is any good.
I use a Whiteside 1 1/4" mortise bit. Cost me $20.00 All I use it for is surfacing. Sharpen once then replace.
If I surfaced wood on a regular basis I would get a different bit.
For surfacing wood (and your spoilboard once you know FOR SURE that your Z is right) Use Paco's surfacing routine. A quick search on this forum will turn it up in a heartbeat.
Which way you go on the bit is personal. All work just fine.
FYI: the reason for using SB's routine for surfacing most often is that the results (hopefully not ridges) will confirm that your Z is good. Pacos just goes back and forth in the x direction so is good for surfacing with the grain. It also does your spoilboard faster than SB's

[jim_rutske]

Chuck, I have opted for a 1.5 inch straight bit from Woodworkers Supply. They are around 35-40 dollars. I am on my second one in a couple years. When it gets a little dull I just take a diamond hand sharpner and put a newish edge on it. Given its large size, sharpening is easy. I not only use it for surfacing the spoilboard but have also used it in flattening/planing rough lumber. My first one got eatin up by surfacing dirty/sandy cedar for a sign. A 'bit' of a lesson there. :o

[Gary Campbell]

Chuck...
I have surfaced a lot of large lumber pieces over the last few years. My first was a 3' by 4' oak table top. The 1 1/4 surfacer I had lasted almost thru the first pass. Many woods, especially the exotics, are oily, which gum the bit slightly, which creates heat, which immediately dulls the bit.

That is why I switched to the Amana 2 1/2" insert cutter ($250+) They are a good tool, and like all good tools, are not cheap to buy, but in the long run much cheaper than soldered carbide bits. The insert bits also seem to have a cleaner angle of attack than the ground bits and shear the wood much better. For spoilboard surfacing it doesnt make a whole lot of difference, other than time. The big bits cover ground a whole lot faster. Like Dave says, your Z axis must be perpendicular to the table in both directions.

[bleeth]

Hey Gary:
You have always run PRS's. I'm not sure that big puppy would be right on a PRT. As you know they are not nearly as smooth and the huge width of that one could be an issue on a PRT gantry. I would keep it to a smaller diameter.
(Note to GC: Issue spoken about earlier solved-fix was too easy-time to Black Viper the thing.)

[myxpykalix]

Chuck,
I guess you need to ask yourself how much use you will give one of these bits in order to figure out what is best for you. If you are like me and only use the bit to surface your table and/or a few other occasions I would go for the magnate 1.5" bit for $22.57
http://www.magnate.net/index.cfm?event=showProductGroup&theID=136
Because it will last you long enough for your needs.

However if you are like Gary or Dave and need to use it all the time then you might want to go with some of their suggestions. I just couldn't see paying $160.00 for a bit that you use occasionally.

[srwtlc]

I've used a 1.5" Jesada for several years for the spoilboard and some surfacing of wood. I've had it sharpened several times and although it may not be 1.5" anymore, it still has carbide to spare for more sharpening. Sharpening cost for me here is about $5.50 each time.

I have a 1.5" CMT waiting it's turn. ;)

[beacon14]

I'm with Gary, and yes Dave, on my PRT (alpha) I use the 2 1/2" insert bit from Amama. Mine pre-dates the newer four-insert variety and has just the two inserts. I also use it to surface hardwoods including exotics and can usually go up to 1/8" deep per pass with a 2" stepover at 4ips, sometimes a little slower in difficult or hard grain or wood with knots. They make different inserts for hardwoods and softwoods (like spoilboards) but I've just been using the hardwood inserts lately and my spoilboard doesn't seem to mind. I re-surface .01" deep at 8ips.

My Z axis is deadly accurate - there are no tactile ridges on my surfaced spoilboard.

Once you are re-surfacing every couple of weeks the difference between a 1" stepover and a 2" stepover saves a lot of time over the course of a year. But you do have to be real careful not to drop them on the floor or run into such things as your brand new pneumatic stops:eek:.

I also think we do less sanding with the surface left by the insert cutter than we used to with the planer bit, and it's nice to be able to put fresh inserts in for the last critical pass instead of making the last pass when the bit is at its dullest.

[frank134]

I am also with Gary,Dave and David. I think the amama 2 1/2" bit is great. But I learn something new here again. I didn't know you could get differance bit or cutter for it. Thank David for the info. I surfaced a lot of hard white maple with it. all of it trun out great.

[waynelocke]

I use a Hersaf 2" insert cutter, http://www.hersaf.com/shop/index.php/action/item/id/215/prevaction/category/previd/7/prevstart/0/subid/14/, which now retails for about $130 plus about $10 for the arbor. I have used this for years. It works great.

[bleeth]

Thanks for posting your experience with that bit David. Having seen your big slab tables if you say it works on your PRT then I will cease to question it (with the added comment that I KNOW your z is adjusted sweet.)

[dhunt]

I am also with Gary,Dave and David. I think the Amama 2 1/2" bit is great.
We use the 2.5 inch dia. Amana bit as seen at
http://www.amanatool.com/cncroutingdetails/rc-2257.html
-the one with two cutter inserts

[Chuck Keysor]

Thanks again everyone for your informative comments.

a) Seeing that there is such a wide cost range in table surfacing options is a bit of a surprise. Prior to my posting, I had thought the 1 1/2" Amana RC-2250 was the top of the line, which made me a bit leary. Somehow, knowing it is a more middle of the line approach makes me feel a bit less guilty about buying it. It is on sale at the moment for $169. (The special sales price I found for the RC-2257 2 1/2" bit was $251.)

b) There were a couple of comments about needing to have the Z axis be perfectly square. I have attached a photo showing what I did a few months back, when I was squaring the Z axis. I hope the picture is clear enough, but I had an 8 foot level laying across the steel bed supports, and then used a full sized framing square laid on the level to establish the fine tuning of the Z axis. I hope this approach will prove to have been successful.

Thanks again, Chuck

[Gary Campbell]

Chuck...
As most of the guys that use them (the large diameter bits) say: You'll know after a few passes! :)

[Chuck Keysor]

Focusing on the Spoil board surfacing bits with replaceable cutter blades, 1 1/2" 4 blade versus 2 1/2" two blade :

The 1 1/2" 4 blade surfacing bit ($169), requires two different types of cutters. So to buy the minimum of 10 of the two required blades adds on another $86, bringing the total price for the 1 1/2" surfacing bit to $255.

The 2 1/2" 2 blade surfacing bit ($251) of course only uses a single blade type. So to add a set of 10 replacement blades adds $34, bringing the total price for the 2 1/2" surfacing bit to $285.

I have hunted all over the Internet, and can not find any actual user reviews of either of these blades. So it makes it impossible to make a wise decision. But several of you have said you use the 2 1/2" two cutter design. Do you detect any problems with the end result of this bit? Off hand, I would not be needing a perfect finish. One would guess that surfacing could get done much faster with the bigger bit. But, for all I know, the 4 blade bit can be used at a higher feed rate. So the bigger question would appear to be is the larger diameter 2 1/2" surfacing bit worth the extra $30?

(Note, I just bought the Vectric Aspire software yesterday, so my wallet is still reluctant to spend any more. But I want to be set up with the correct equipment,,,,,,,)

Thank you again, Chuck

[Gary Campbell]

Chuck...
The insert cutter I have uses the 12mm 4 sided insert. They work great. There are thousands of this same insert in "Shelix" cutting heads on planers and jointers all over the country.

You were looking all over the internet and forgot to read this post! There are a number of experienced ShopBotters above that are giving a good review to these bits. There are also a few more that give some cost saving alternatives that, according to them, perform well. How much info do you need? :confused:

We gave the best review of all: We voted with OUR checkbook.

EDIT: Forgot to mention.... I bought mine in 2007 and I have used only the original 2 and 6 more inserts from my first box. Spoilboard is sufaced almost weekly, slabs are surfaced fairly often. Another review (slightly different perspective) http://www.talkshopbot.com/forum/showthread.php?t=13458

[Chuck Keysor]

Thanks Gary. I was assuming that because the 4 wing cutters are something new, that they may have some significant advantage when compared to the older 2 wing cutters. I was looking for reviews of the new 4 wing cutters, so that I might compare that design to the already good reviews given here on the two wing cutters. That way I hoped to see what I might be trading off by stepping up to the larger size 2 wing cutter.

And, on a deeper level, getting caught up in the details gives me an added reason to hang onto my cash a little longer...:o

[Gary Campbell]

Chuck...
The 2 styles have both been around as long as I remember, so I dont really think the 2+2 style is really that new. Maybe for some brands. There may be some advantage to the 2+2 design, but is unknown to this group.

I fully understand about "moving at the speed of cash", but then a surfacer is one of the first bits you will need. Try one of the less costly alternatives listed above to start. Very few will buy these bits first, unless they have a good sized tooling budget or a impending job that requires them. Another cliche would be: "pay me now, or pay me later"

[beacon14]

If you are in it for the long run the 2 1/2" bit is worth the extra $30. A box of 10 cutters will last you a good while.

Only downside I could see is that if you just can't get or keep your Z axis square you'll have bigger ridges with the wider bit.

[bleeth]

Readings from a bubble level are not the right way to square your z.
You can do it with a digital level but the best way to check it is to put a trammel in the chuck and check it with a feeler guage. This has been written about on the forum many times. I also think it was written up in one or two of the articles on the SB site written by botters.
Forgive me for not supplying links. I prefer to offer guidance rather than leading by the hand.

[donchandler]

Dave is right, you can not even get close to squaring the Z axis with a level.
I have an L shaped bracket that goes in the chuck. The short leg of ( about 3") the L goes in the chuck. The long leg ( about 10") has a dial indicator on it. Touch the indicator to the table and rotate the chuck by hand 360 degrees. You will see the high and low side. Adjust the Z axis until you can rotate it and the indicator doesn't move more than a couple of thousands. The closer you can get it, the better off you are.

[Chuck Keysor]

Thanks again for the replies. I did use a Wixey digital gage in my table set-up. For what it is worth, I have attached a picture that I posted here back in the end of March.

However, I did find what seemed to me to be a higher degree of certainty in my readings by combining the digital meter with the level. Because interestingly, with an 8 foot level, it is possible to raise one end visibly and see a change in the vile, while not changing the reading on the Wixey at all. So I worked the level together with the Wixey to resolve where the real zero of the Wixey was. Or at least that is what I thought I was doing.:confused:

The 8 foot level on the bed was not for leveling purposes, even though it read level, with the Wixey on it. It's purpose was to serve as a straight edge, that would average out the variations in center height of the horizontal bed supports, as oddly, at the center, they were not all on the same plane, even though they were where they met the side rails.

As to the trammel measurements, I bought an "A-Line-It Deluxe" dial indicator over a year ago, to use for my ShopBot. However, I haven't used it, because my spoilboard hasn't been planed yet, which I had understood (or mis-understood) to be a required prerequisite.

In any even, I did order the 2 1/2" Amana (2257) surfacing tool, so if I have my Z axis all screwed up, I will find out soon enough, and wade into that.

Sorry that I pulled my thread off its original topic of the spoilboard flattening tool. That was all I really was after, and the z axis topic came up innocently enough based on someone's concern over the effect of a large tool upon my spoil board if I didn't get the Z axis trued accurately.

Thanks, Chuck

[tgm]

In this day and age using a cutter threaded on to an arbor is like going back to the '40's. It reminds me of the **** that Sears used to sell for the home hobbyist, router bits with threaded shanks. Why today would anyone still make them with all the cutter technology that has been developed over the years is beyond me.

Buy one of the one piece, replaceable insert units and you won't be disappointed.

[waynelocke]

The HerSaf bits are quality, industrial bits, several which I have used for a long time. They are well balanced, have no vibration and the inserts are easily changed. They bear as much in common with the Sears bits, which by the way I remember, as the router bits of the 70's have with a "Spiral O". Hey your car has four wheels, it must be the same as a 1949 Chevrolet.

[rhfurniture]

fwiw, I use an 80mm (3.5") insert tooth cutter from Carbitool (Australia) in my 3hp spindle and it works a treat at 12krpm. I wish some of the other big tooling manufacturers made large insert cutters (eg adjustable bevel) with 16mm shanks.
R

[rhfurniture]

fwiw, I use an 80mm (3.5") insert tooth cutter from Carbitool (Australia) in my 3hp spindle and it works a treat at 11krpm.
R

[Chuck Keysor]

Hello. I used my new Amana 2 1/2" dia surfacing tool, and got mixed results, in that I don't get any ridges cutting in the x direction, but I do in the y direction.

Using a dial indicator and a trammel set with a 6 inch radius, and a clean piece of glass, I took dial indicator readings at 0, 90, 180 and 270 degrees. The nature of these readings is shown in the attached photos.

When I started out, my spindle had only been squared with a square and a level. I surfaced the spoil board, and with the spindle center at x=10", y=15", I made the following readings:
0.000" at 0 deg, -.005" at 90 deg, -.005" at 180 deg, +.004" at 270 deg
I got perfect cuts (no ridges) going in the x direction, but small ridges going in y.

I spent a couple of hours, trying to shim my spindle into perfection (0.000" at 0, 90, 180 and 270 degrees). The spindle was centered on x = 10", y = 15". I finally had to give up with readings of:
0.000" at 0 deg, -.002" at 90 deg, -.003" at 180 deg, -.002" at 270 deg.
Again, I got perfect cuts in the x direction, but small ridges going in y.

Further study showed at near home, lower left corner of the table, I had no ridges at all, and the area of about one square foot was absolutely perfect. But as the cut progressed to the back of the table (in the y direction), the ridges appeared, and grew in proportion to the distance from the home position. The ridges at the middle of the left edge were very slight (visible and could be felt). And, while larger at the back edge of the table, they were still very small, and sand off easily.

So, I made my trammel mounted dial indicator readings, at home, middle of left edge, and the back of the left table edge, to see how they reflected the size of the ridges.

At x=10, y=10, I measured:
0.000" at 0 deg, +.005" at 90 deg, +.012" at 180 deg, +.006 at 270 deg.

At x=10, y=30, I measured:
0.000" at 0 deg, -.001" at 90 deg, -.006" at 180 deg, -.004" at 270 deg.

At x=10, y=50, I measured:
0.000" at 0 deg, -.005" at 90 deg, -.011" at 180 deg, -.003" at 270 deg.

Do these readings make sense to anyone? Do they provide any clues as to why I have my ridges going in the y direction, and that they grow from nothing at the home position, and increase linearly from there? Do I just have to live with these? Even the worst sand off easily.

I will note that making the adjustments with shims to plumb the spindle is very difficult, and everything is very interactive with each other. And, even if I lean on anything anywhere, the slightest amount, the dial indicator readings change noticably. So the system is mechanically very delicate, and I wonder if my ridges are changing as a function of the spindle sagging the gantry. But then my ridges should be symetric around the middle of the y axis, and they are not.....

Last note, I typed all this up very laboriously, then went to post it at 1:15am, and it all just vanished. So I had to retype it all, sigh........ It is now after 2am.........

Thanks, Chuck

[bleeth]

The issue is probably in your Y rails. They are not consistantly level with each other and therefore your z is not staying plumb as the carriage moves.
Easiest way to fix is to use a digital level and shims.
Also check that they are each individually flat with a proper straight edge (a milled steel one is best).
After quite a bit of use I ended up capping mine with hardened rails to get them flat as they were worn somewhat unevenly and one was also a bit bowed.

Also note that mechanical inconsistancy and flex in the PRT gantry is what led to the PRS design. Eventually I simply rebuilt my gantry to a PRS.

[Gary Campbell]

Chuck...
Yours are predictable results. I suggest:

Find a surfacing routine that only surfaces in the X direction as most of us have. The 4 direction routine from SB exaggerates any error or flex that is present. A 2 1/2" bit adds to visible error. Do a forum search, there have been routines posted by David Buchsbaum and Paco that are the basis for my current ATC surfacing routine.

Your worst case (.012 over 12") is only 6/100 of a degree.

Snug all your V rollers and go have fun with your machine. Dont worry about your findings until NASA calls and needs some high tolerance parts.

[Brady Watson]

Getting the Z dialed in can be very illusive - but I assure you that when you 'get it', you'll know how to precisely adjust the Z to achieve a perfectly flat surface with no ridges.

Remove the shims. They are never necessary on the Z axis. (I didn't believe this either...at 1st) First, make sure that the v-rollers on the Z axis are tight to the t-rail & that the Z rack & pinion have a good mesh without excessive lash. You have a heavy 5hp spindle and you only have 4 v-rollers on the Z. Your tool was only shipped with 4, but you can see there are provisions for 4 more v-rollers - you can see the holes where they would go. Definitely worth getting as they drastically reduce t-rail wear & stabilize the Z.

Move the Z down where the cutting takes place - as if you have your flattening bit on the spoilboard surface. Wiggle the spindle all around. Feel any slop? (Make sure control box is on) Where is the slop coming from?

If you don't feel any slop & the Z is tight, you can use a bit of English with a rubber mallet at the top of the t-rail to influence the Z tower in the X direction. Read the ridges and they will tell you which way the Z wants to go. If you need to adjust in the Y direction, you'll have to loosen the Z tower bolts. Take the shims out & snug the L brackets up to the strut. Then loosen the Z tower to L bracket bolts. Just snug the bottom bolts, which will let you stabilize the Z a little as you adjust. A level will get you really close if your table is leveled properly. Dink the Z with a mallet to dial in. CAREFULLY snug up the Z tower to L bracket bolts - GINGERLY - a little at a time, like you are torquing a head on an engine - little here, little there EVENLY. The Z will go out of adjustment if you pull it one way or another.

You WILL get this figured out...just be patient. Dial indicator is not necessary. Just read the lines on the spoilboard - they will tell you what you need to do. Now would also be a good time to clean the rails of debris & deburr if necessary. Be sure to observe the horizontal V-rollers on the Y car to make sure they don't 'ride up' the sides of the rail as you move from Y0 to Y48/60. This can also cause the Z to lift and give you weird results when trying to read the lines...

-B

[beacon14]

Use a larger trammel and put the dial indicator away. I use a trammel that's about 18" long with a pencil in the far end, so I swing a 36" diameter circle and just watch how close the pencil comes to the table all the way around. At that size if the pencil tip just touches at its lowest spot, and leaves a gap of no more than 1/16" or less at its highest point, all is good.

A large trammel, following Brady's suggestions for tweaking the Z axis, and Gary's suggestions for surfacing in one direction only, is the ticket. Assuming, that is, that you really need it to be any better than it already is.

[Chuck Keysor]

Thank you all again for providing me so much detailed, targeted information relating to my PRT alpha's alignment issues. I have located and downloaded Paco's flattening routine, and will try that out tomorrow. And I will try and correlate your observations with my machine.

I am trying to balance off various objectives with getting my machine going. And from the general tone of your replies, it would seem that the mechanical issues with my machine are not earth shattering, and can be dealt with outside of the "critical path" of getting my machine up and running. So I will be getting back to the study of my Aspire software, which is truly in my "critical path".

Thank you again, Chuck

[Chuck Keysor]

Overview: Paco's flattening routine doesn't seem to function correctly for me. What am I doing wrong?

Details: I downloaded Paco's flattening routine, mostly to see if my previously discussed ridges would show up when flattening some rough lumber. I tested this on a crooked piece of rough sawn oak, that was 3 inches thick, 27 inches long and 8 inches wide. My jointer is only 6 inches wide, so I thought this would be a useful test.

When I ran Paco's routine, it of course asked me to fill in if I wanted to cut in the x or y direction, the dimensions of the lumber, the size of my cutter, step-over and depth of cut. I was expecting that since it knew the width of my board, that it would make one pass, then move over about 2 inches, then take another pass, and after 4 passes be done, and ask me if I wanted to make another set of passes to remove some more material.

But when I ran the routine, it would only make one pass, clearing out a 2 1/2" wide path, and then stop. I played around with it trying to enter different values, and in the step over percentage, I first used .1 for 10%, but in a later trial, I entered 10 for 10%. But there didn't seem to be much else that could be wrong. What am I doing wrong? :confused:

(I did one side with Paco's routine, and resetting the cutter position, to shift each additional pass to a higher value of y. That was really teadious. The other side, I cut faster by just using the keypad to move the cutter. But while much faster, it was still a pretty dumb way to flatten my oak!)

Thanks again for your help. Chuck

[Gary Campbell]

Chuck...
When it asks for the stepover, try putting in a number between 1 and 2 inches. (assumes 2.5" bit) (You assumed a percentage)

[Chuck Keysor]

Gary, I ran Paco's flattening routine again. This time for step-over, I entered 1, then 1.5, then 2, then 3. In all cases the ShopBot ran the little ramping sequence, then a single cut pass, and then stopped. With the width of board and the 2.5 inch cutter, there should have been 4 passes to cover the full width of the board.

Also, in the data entry window that asks for the step-over value, it says percent.

Again, I need to have an application for flattening rough lumber. But I also need to check out my 2.5" cutter and see how well it works with the present alignment of my machine.

Any suggestions for making Paco's application function as I expect? Thanks, Chuck

[ken_rychlik]

Why don't you just make a rectangle in aspire a little larger than the board you want to surface and make a pocketing toolpath for the the box. It's very simple to do.

I have even made spoilboard surfacing files this way.

If you choose raster it runs faster on the machine, but with offset it will tell you more about how square your z is.

[srwtlc]

Chuck,

Try your initial settings with 65%. That should give you about 5 passes. Works in preview for me with your settings. 10% will only give you about a 0.25" stepover.

Maybe your "Paco's Surface" file is corrupt. I can't remember if I made any modifications to mine, but here it is if you want to try it.

[Chuck Keysor]

Thanks again for the replies. I down loaded Scott's version of Paco's flattening file, and ran that. I chose to cut in the x direction, the board was 20 inches in x, 10 inches in y, cutter was 2.5 inches, and I used step-over from 75, down to 50, down to 10, to .75. In all cases, the cutter made its little plunge entry, and then one single pass in the x direction.

Even if these values were all wrong, I would have guessed that it would try to keep making repeated off-set passes until it had covered the full width of the 10 inch board. When it just makes one single pass and then stops, something has to be out of whack. But Paco's intereface seems so simple, it is hard to imagine what I messed up. And to show my set-up isn't totally out of whack, using the table surfacing routine from the Shopbot tool set worked as expected.

I guess I will follow up and try the pocketing routine. However, I have just been watching the Aspire videos, and after the introduction to the interface, everything, for hours, is about making signs, and related operations. I didn't see anything in the index about just basic machining operations. A few years ago, I took some Mastercam training, and all of that was about basic machining operations, with scads of different types of tool motions, with and without lifts between passes. The point being, it seems as though even pocketing and basic machining operations in Aspire should have detailed instructions. Is basic machining covered somewhere other than the video lessons?

Thanks again, Chuck!

[Brady Watson]

Chuck,
As you are finding...there are many ways to generate a flattening file. It all boils down to A) What is easiest for you and B) What gives you the best result.

Here are a few options:

1) Use the CR command with pocketing feature. (be sure to check VC 1st)

2) Under tools in SB3, choose the Tabletop Surfacer tool. It is an easier to use CR command.

3) Create a rectangle that is 1 tool diameter wider and taller than the size you are surfacing. Then in PW, Aspire etc create a pocket toolpath. You can choose offset or raster depending on your grain, if necessary.

4) Draw a straight line 1X longer than your tool diameter & center it on the material. Then block copy the line in Y 0.6 times offset the diameter of your tool. Alternate start points on the line to create your own raster toolpath.

Hopefully you have gotten your machine dialed in. You are always going to see lines where the cutter has been - but you should not be able to feel any ridges. If you do, you need to dink the Z in the direction the ridge angle tells you it needs to go.

-B

[Chuck Keysor]

Thank you Brady for giving me an overview of the different techniques which are available for me to flatten my boards! I had no clue about these options, due to my still very limited operational engagement with my ShopBot. Such insights as you offered can only come from a deep understanding of the machine and how it can be used. Again, this is why I am so thankful for your assistance, and of all the other users who help out we beginners.

As to my ridges, my cuts in the X direction are flawless across the entire width of the machine. There are no ridges that can be seen or felt. There is just the interesting effect that as the big cutter moves, in one half of its diameter, it is cutting in a conventional direction, and the other half of its diameter it is climb cutting. This leaves a surface texture effect that is visible, understandable, unavoidable and acceptable!

Thanks again Brady. Chuck

[Brady Watson]

No problem, Chuck. You're welcome.

Yes - the climb/conventional marks are a fact of life. There will always be a little bit of 'texture' as you put it.

-B