Sanity check on aisle Onsrud!

[geneb]

I've got a pair of Onsrud 64-025 cutters that I just purchased - they state the cutter diameter as .25, but my caliper tells me .235. Is there anyone here that has one they can check for me? I'm either losing my mind, my caliper is, or Onsrud's part specs can't be trusted. :(

tnx!

g.

[scottp55]

Gene, Just curious. Directly from Onsrud? SB starter set .125" straight was .1135" which sent the machinist who was helping me through the roof! He convinced me to set up my "ACTUAL" category which has saved my butt more than once. I've got a couple suppliers who are Consistently .005" undersized and I can go through dozens of their bits without finding ANY discrepancies.
I Always measure now, and keep "Currents" in a separate box until I go to use them.
Just mucked me up yesterday.
If I see "Onsrud" I measure it! Very good cutting edges, BUT dimensions are ALWAYS in database in Actual and carefully monitored and a fair amount of discrepancy between Kirks Database and mine! Hard to exchange files when common bits are different diameters. We always have to make sure he's changes bit to HIS Database. Pain!!

[Burkhardt]

But that is a single flute cutter. How do you even measure the diameter at the flute with a caliper? You can not lean both jaws of the caliper against a flute edge.
If you just measure against the opposing surface, this is definitely undercut to not rub on the material. Or did you measure the shank diameter?

Maybe you can cut a clean slot in dense hardwood and measure if it is actually undersized?

http://www.onsrud.com/productImages/64-025/250x250/1.jpg

[Brady Watson]

Maybe you can cut a clean slot in dense hardwood and measure if it is actually undersized?


This is the ONLY reliable way to tell...

-B

[ssflyer]

I've found MDF to work well - just measure it right after cutting...
It's cheap!

[geneb]

I was rotating the cutter in the jaw of the caliper. I'll do a test cut and see how it works.

tnx.

g.

[MogulTx]

I've rotated the bit in my caliper, but I find the actual test of the bit to be the reliable method. I try to cut in the material I am going to work with and at the roatation and travel speeds that I'd like to use- which gived me real world information from which to assess my cutting project

[jTr]

I've found the under size issue to be true on any brand bit if measured with a caliper, regardless of physical limitations and variables discussed above.

To consider:
- Shank is very likely precise at .250 , being pulled from carbide tool stock
- in order to shape and sharpen, it is inevitable that you'll loose some material
= Average of .005 to .006 under size is to be expected, and quite amazing, really.

When is this a significant issue?

For me, it is dados. When using melamine, it can be dead on for a 3/4" material. As of late, my suppliers seem to run upwards of .015 over size. In generating computer shop drafts of cabinets and furniture, it is done with the assumption of exact material thickness, which is obviously never the case for the sheet goods.

How to cope?

Under-size dados with under size plywood = very acceptable results, and I've ceased burning energy worrying. I'm making cabinets, not engine parts. A fit with .015 wiggle room makes for smooth assembly, and no excessive gaps in critical locations upon completion.

Under-size dados with over size melamine = now I'm sweating. My current formula:
.005 under size bit makes a pocket that is .010 under size, since I'm loosing .005 on both sides of the cut.
.010 to .015 over size on melamine = .020 to .025 under sized dado for a proper fit.

As of late, my solution is to assign an offset of +.021 on the pocketing tool path for the dado layer in Part works/ V-carve Pro.
This typically results in a super-snug fit that is more urgently required with melamine.

Adjust according to results you are getting, and if frustrated, remember, this is far easier to remedy in the CNC world than dealing with dado blade shimming in a table saw!!!

This seems a good place to interject an oft - stated but important note: Be sure to use a down spiral for any pockets cut into sheet goods, especially melamine. Tool change to compression bits for profile cutting, and be certain your first pass plunges .030 to bury the up cut tip into the material, assuring the down cut flutes are hitting that delicate face.

Jeff

[Justin G]

I've found the under size issue to be true on any brand bit if measured with a caliper, regardless of physical limitations and variables discussed above.

To consider:
- Shank is very likely precise at .250 , being pulled from carbide tool stock
- in order to shape and sharpen, it is inevitable that you'll loose some material
= Average of .005 to .006 under size is to be expected, and quite amazing, really.

When is this a significant issue?

For me, it is dados. When using melamine, it can be dead on for a 3/4" material. As of late, my suppliers seem to run upwards of .015 over size. In generating computer shop drafts of cabinets and furniture, it is done with the assumption of exact material thickness, which is obviously never the case for the sheet goods.

How to cope?

Under-size dados with under size plywood = very acceptable results, and I've ceased burning energy worrying. I'm making cabinets, not engine parts. A fit with .015 wiggle room makes for smooth assembly, and no excessive gaps in critical locations upon completion.

Under-size dados with over size melamine = now I'm sweating. My current formula:
.005 under size bit makes a pocket that is .010 under size, since I'm loosing .005 on both sides of the cut.
.010 to .015 over size on melamine = .020 to .025 under sized dado for a proper fit.

As of late, my solution is to assign an offset of +.021 on the pocketing tool path for the dado layer in Part works/ V-carve Pro.
This typically results in a super-snug fit that is more urgently required with melamine.

Adjust according to results you are getting, and if frustrated, remember, this is far easier to remedy in the CNC world than dealing with dado blade shimming in a table saw!!!

This seems a good place to interject an oft - stated but important note: Be sure to use a down spiral for any pockets cut into sheet goods, especially melamine. Tool change to compression bits for profile cutting, and be certain your first pass plunges .030 to bury the up cut tip into the material, assuring the down cut flutes are hitting that delicate face.

Jeff
I have been making a lot of plywood puzzle parts as of late, with perpendicular joints using dog bones so everything merrys up flush. Well every time I cut the parts with the exact width of the material measured with digital calipers, they don't fit, too tight. I was freaking out, thinking the bot was losing accuracy or aspire was f'd somehow. so I kept doing this negative offset in the profile passes. trial and error and so frustrating. Now I totally realize its because of the bits being smaller than their actual labeling. DUH! of course they are. Now i'm going to go insane trying to figure out how to measure my ballnose bits.. eesh.

[Brady Watson]

Wait a minute...End mills are most certainly their advertised size +/- 0.001 or so depending on where you get them. They are certainly not off by 0.005" - no way.

If I drill a hole with an end mill it is as close to exact advertised diameter as my digital bore scope or plug gauges can measure. 2-flute upcut spiral router bits are not typically manufactured to the same tolerances as metalworking end mills - but Onsrud is a good outfit and should be to spec.

Wood moves around while being cut. Dados can cup or be off-spec because your chipload wasn't right (EG - cutting too fast)...they can be WAY off by leaving the default Climb mill selected instead of Conventional when doing dados and pockets. A simple mouse click may cure all your ails.

-B

[jerry_stanek]

I am not sure what brand bits I got but they were stamped with the correct size on them IE .25 stamped .245

[Ajcoholic]

When I bought my machine I bought nearly $4000 in tooling from Onsrud (mostly various end mills ,ball end mills, etc in various sizes lengths and up/down spiral), as well as a whole lot off their eBay clearance site.

I cut a lot of grooves and dados and never have had issue.

I purchase other cutters from BC Saw & Tool, and Royce Ayr as well ( both Canadian manufacturers) which also seem very accurate.

I'll mic some of my Onsrud bits if I can remember to do so, just for curiosities sake.

[Justin G]

I could have my procedures just completely messed up, I am fairly new to this whole thing, but this is what I do.

cutting 1/2" baltic birch ply, using an onsrud 1/4" downcut spiral. I cut through the material in one pass CLIMB cut. my F&S are based on sound of cut and heat of bit afterward. Which translates to 3.5 IPS F and 7500 rpms on the spindle. I then come around again with a negative offset something like .004 and same F&S but using a conventional cut. This is using an outside vector profile cut and aspire.

Its important to note that when making puzzle pieces where the surface of the material is parallel with each part, I literally copy and paste the same vector on two different interlocking pieces. I figure the negative offset of .004 (.008 cumulatively) will make everything have a little play and fit nicely. Sometimes they fit, sometimes they do not.

For my pieces that are perpendicular, I do everything the same, except I get the distance of the dado from my digital calipers measuring the thickness of the ply. I know that ply thickness is not consistent, but how much could it be off by? I always make the dados bigger to leave room for paint and such, and still they do not fit sometimes even with a .0156 increase in size.

I have yet to measure the actual width of a single pass for each given tool, like Brady mentioned earlier, but I did measure the width of the dado while the cut file was going on before I removed the material from the table, and that is how I found the correct negative offset to fit the parts.

Is it possible that when cutting through the material, it somehow is ever so slightly pulling the plys apart?

[Justin G]

Here are a couple pictures for clarification.

I will be testing my cuts today in both climb and conventional directions on some jatoba hard wood to see channel width.

[Ajcoholic]

Wood is funny stuff - unlike metal where you can have a slip fit with just a few ten thousandths clearance, I find with fitting either solid or sheet material into grooves etc, 5 thousandths clearance is the sweet spot.

Even if I carefully set up a groove on my shaper that measures the exact thickness of the sheet stock, if at least 4 to 5 thousandths is not allowed for clearance the fit is too tight.

Same as with the CNC. If I machine a slot to accept the exact ply thickness it is always too tight

I run a lot of grooved framing, etc and doors - all my working career I've tried to hit that 0.005" clearance. Works for me...

[Simops]

This thread has intrigued me. So I decided to test two of my 2 flute down cut bits by cutting a 3/16" deep groove 5 inches long. Using same conservative feed and speeds for both with conventional cut.

Onsrud 57-910 (as used in the SB starter kit) recently purchased and sharp.....measured groove width 0.245"

Amana 46-348 (new bit) ..... Measured 0.247"

Using the 57-910 bit I outside profile cut a 2.5" square (again cutting as above) using 1/2" ply with two passes. The resulting square cutout was exactly square but measured 2.57" in X and Y.

I then cut a wider dado to fit 9mm AA ply (ply here is metric) .....equivalent to your 3/8" ply measuring 0.355" nominally.
Again using conservative cutting ....nothing hard. The pocket was drawn dxactly 0.355".
After cutting I measured the dado and it was too tight to fit (measuring 0.348)
So recut using 0.425 and it fitted this time although tight.

So the 1/4" tools measures 0.005" undersize. Never considered this significant but I guess when cutting precisely it does and so I will edit my tool database to account for the undersize and see if that makes a difference when I cut my 2.5" square block. It's late Sunday night here so will try tomorrow.......

Cheers

[jTr]

OK - I'm intrigued as well - I posted on this in July, and made some bold statements, (and maybe a rash assumption):o, so I'm taking a second look at my Bits:

Whiteside brand .375 down cut used for dados/rabbets:
Shank diameter: .374. When measured at tip, two flute, spin in caliper to settle in without catching the flutes, still reading only .368-.369.

Centurion brand .25 compression, 2 flute also:
Shank diameter .249. When measured at the tip, same method as stated above: .247.

Perhaps I need to go to Centurion or Onsrud for my 3/8 bits. The variance in the Whiteside brand definitely shows up in undersized pockets. One would think this brand would be more exact - They certainly are not a low price leader for professional tooling...

Next step: do the test cuts. Very curious to see how the measurement from the cutting edges relates to the actual kerf being produced. Admittedly, measuring across the cutting edges is not likely to be the most accurate, but worth noting shank diameter vs. cutting edge should come out much tighter, as with the .25" Centurion.

Glad this thread was resurrected - curious to see other's results with the kerf test, and I'll post mine as soon as I get a chance to run it.

jeff

[Simops]

...............
So the 1/4" tools measures 0.005" undersize. Never considered this significant but I guess when cutting precisely it does and so I will edit my tool database to account for the undersize and see if that makes a difference when I cut my 2.5" square block. It's late Sunday night here so will try tomorrow.......

Cheers

Well I can understand the title now....Sanity! Because my Sanity was tested today. After a couple of hours of numerous cuts I wasn't getting any sense of this....

From my earlier post I found the Onsrud 57-910 down cut bit was 5 thou undersize.....and therefore maybe reason for my 2.5" square test to be oversized....by about 7 thou or so.
So I went today and edited my tool database and put in 0.245 as the tool diameter.
I recut the square (using 12mm MDF = 0.478") with outside profile cut (3 passes) and the square was about 10 thou undersize...Huh...what gives?

Anyhow after numerous cuts varying the tool diameter I ended back at 0.25" and found that the direction of cut was crucial to the accuracy I can achieve.
What I found was as follows:

1. Outside Profile Cut of a 2.5" square:
Tool diameter 0.25" speed 14K Feed 2"/sec, 3 passes (conservative cut so as not to deflect bit).
Conventional Cut = exact 2.5" square.......but
Cut as Climb = 2.518" square. That's 18 thou oversize!!

2. Dado using Pocket cut to fit the 12mm MDF (0.478"). Tool diameter F&S as above.

Draw the dado as 0.478 wide.
Cut as Conventional = 0.47.....8 thou undersize and tight....could force it in.
Cut as climb = 0.458....wow!!!! 20 thou under.....way too tight.

So taking Andrews advice above I added 5 thou to the dado widthin Aspire.....making it 0.453"
Conventional cut = 0.477"......1 thou under but OK fit.
Climb cut = 0.465" ..... Too tight.

So with Pocket cuts I cannot get accuracy with fit without oversizing the dado by at least 5 thou but only with conventional cut.

It's clear that I have to use Conventional cut strategy to get any sort of accuracy. Climb cuts are horribly undersize by around 20 thou with pockets BUT around 18 thou oversize with outside profile cuts......Maddenning!

What gives here? Why use climb cuts? They don't seem accurate enough in my case anyway. Although I have worked out that I need to use conventional every time I do cuts but why?

I could go further with tests using other bits but I was going crazy and gave up for now!

Cheers

[joe]

I'm with Brady!

Joe

[Simops]

Yep Joe I agree...what Brady and Andrew say is somewhat true....
But my downcut end mill was checked by making a groove and it IS 5 thou under not a thou as Brady says. And yes using Convetional cut as Brady says is what I found as well .....so when do you use Climb? Why is it the default selection? What's the point of using Climb if is going to give inaccurate cuts?

Also what Andrew says is true to.....add another 5 thou and the dado cut is spot on but only because the pocket is still undersize, yet outside profile isn't.......it's the inconsistency that gets me......ho hum......will have to do a few more tests and write down all the idiosyncrasies down to remind me when I draw and tool path.......

Cheers

[aschutsky]

WOW! I'm so glad I found this thread. I've been battling with the same issues you guys mentioned here recently, especially when using MDF which is much closer to actual advertised size vs. plywood.

I've been using mostly 3/8 centurion bits and found that the BEST (closest to spec) measurement of the cutters I could get was .371 or so. I hadn't thought of doing a straight cut and measuring. Also, it's embarrassing but I hadn't paid much attention to the climb vs. conventional thing and left that as default. I'm with the others - why they heck is the climb function there if it's not accurate?!?!

[Justin G]

WOW! I'm so glad I found this thread. I've been battling with the same issues you guys mentioned here recently, especially when using MDF which is much closer to actual advertised size vs. plywood.

I've been using mostly 3/8 centurion bits and found that the BEST (closest to spec) measurement of the cutters I could get was .371 or so. I hadn't thought of doing a straight cut and measuring. Also, it's embarrassing but I hadn't paid much attention to the climb vs. conventional thing and left that as default. I'm with the others - why they heck is the climb function there if it's not accurate?!?!
I think the main take away from all this is that no bits, regardless of manufacturers come exactly to spec, and I don't see that as too much of a problem. Doing test cuts is pretty much SOP when working with new materials/ bits so I will be incorporating these cuts into projects from now on.

Andrew, I think there are times when climb cuts are advantageous, 1 reason is that I think it puts less lateral force on the parts being cut. Cutting direction is important when you come to end grain because a lot of times conventional cuts have had a significant tear out for me. I think (again I'm new so everything is still "I think") that is why a lot of more experienced guys and now me, advocate an onion skin strategy where you remove the bulk of material with climb and come back through with conventional.

Something else I read between the two strategies and look at the edge quality of your cut out piece vs the main material, which one is cleaner will tell you which cut direction to use under those circumstances.

[aschutsky]

I think the main take away from all this is that no bits, regardless of manufacturers come exactly to spec, and I don't see that as too much of a problem. Doing test cuts is pretty much SOP when working with new materials/ bits so I will be incorporating these cuts into projects from now on.

Andrew, I think there are times when climb cuts are advantageous, 1 reason is that I think it puts less lateral force on the parts being cut. Cutting direction is important when you come to end grain because a lot of times conventional cuts have had a significant tear out for me. I think (again I'm new so everything is still "I think") that is why a lot of more experienced guys and now me, advocate an onion skin strategy where you remove the bulk of material with climb and come back through with conventional.

Something else I read between the two strategies and look at the edge quality of your cut out piece vs the main material, which one is cleaner will tell you which cut direction to use under those circumstances.

Justin - Appreciate the added insight as to climb vs. conventional. I tried reading through the Vcarve documentation but didn't see much detail there. I'll continue reading to further educate myself, but for now (using mostly MDF) will switch and test with conventional cutting.

[steve_g]

Andrew…
Climb and conventional cutting are two very useful tools in our arsenal… Knowing when to use them is critical to success!
As a bit addresses the wood, a tapered chip is removed. A conventional cutting direction removes this chip from the thin to the thick part of the chip, while a climb cut hammers into the wood at the thickest part of the chip, thus the climb cut isn’t quite as smooth as the conventional cut. HOWEVER the conventional cut is more prone to splintering! Some woods like western Cedar will start a splinter and run it the full length of the board! A climb cut will cut these splinter prone grains off, so it can’t run.
How to get the best cut every time…
Almost without fail, you can get the best cut possible in wood using what is called an “onion skin” cutting strategy. This method Uses both climb and conventional cutting to their best advantage. First, make a Climb cut with about a .01 to .015 allowance. This means you have just a little “Onion skin” of material left to remove to get to finished size. Next, repeat the cut in the conventional direction without any allowance. The cut in the conventional direction can be made full depth in a single pass as only an onion skin of material is being removed. This same strategy can be used on the depth as well as the edges… doing it on the depth leaves a continuous tab in place while the most cutting forces are being used.
BTW… cutting in a raster pattern leaves you reversing cut and climb each pass. This can leave you with tear out in the bottom every other pass, making it hard to sand smooth.
SG

[Justin G]

Andrew…
Climb and conventional cutting are two very useful tools in our arsenal… Knowing when to use them is critical to success!
As a bit addresses the wood, a tapered chip is removed. A conventional cutting direction removes this chip from the thin to the thick part of the chip, while a climb cut hammers into the wood at the thickest part of the chip, thus the climb cut isn’t quite as smooth as the conventional cut. HOWEVER the conventional cut is more prone to splintering! Some woods like western Cedar will start a splinter and run it the full length of the board! A climb cut will cut these splinter prone grains off, so it can’t run.
How to get the best cut every time…
Almost without fail, you can get the best cut possible in wood using what is called an “onion skin” cutting strategy. This method Uses both climb and conventional cutting to their best advantage. First, make a Climb cut with about a .01 to .015 allowance. This means you have just a little “Onion skin” of material left to remove to get to finished size. Next, repeat the cut in the conventional direction without any allowance. The cut in the conventional direction can be made full depth in a single pass as only an onion skin of material is being removed. This same strategy can be used on the depth as well as the edges… doing it on the depth leaves a continuous tab in place while the most cutting forces are being used.
BTW… cutting in a raster pattern leaves you reversing cut and climb each pass. This can leave you with tear out in the bottom every other pass, making it hard to sand smooth.
SG
Great post steve. It is always better for me to understand the physics behind why things work, and don't work.

Andrew,
I'm not sure if you have then, but getting a pair of digital calipers, and digital depth guages saves the day. I use both non stop throughout my day.

[Justin G]

These are what I use:

http://smile.amazon.com/iGaging-ABSOLUTE-Digital-Electronic-Caliper/dp/B00INL0BTS/ref=sr_1_1?ie=UTF8&qid=1420496882&sr=8-1&keywords=igaging+digital+caliper

http://smile.amazon.com/iGaging-AccuMarking-Digital-Marking-Height/dp/B00GBXX9F8/ref=sr_1_1?ie=UTF8&qid=1420497515&sr=8-1&keywords=igaging+digital+accumarking

One for measuring off table, and one for measuring once I have the material mounted to the table.

[Burkhardt]

When you want to judge bit accuracy you only can do this with a slot. But even then, measuring the width of a slot by hand with a caliper in wood which is rather soft and has a fibrous surface is a challenge. I don't think you can get that reliably better than 2 or 3/1000".

If you start measuring the dimension of a cut-out piece like that 2.5" square, you will rather measure the machine flex, backlash and bit flex than the bit diameter. That makes the difference in climb vs. conventional because the machining forces will pull the spindle against or away from the intended path.

For what it is worth, a good rigid CNC router should have a flex of better than 5,000 lbs/inch (easy to measure with a dial indicator and a fishing scale). That means machining or inertia forces of 20 pounds can already move the bit by 0.004" not counting possible backlash.

[Simops]

Good info.....it's good to read the science behind reasons for doing things as it clears things up.......Steve good explained info....(some of the posts by more experienced guys tend to be somewhat scant in basic detail at times for those still learning!!) ....
I read about onion skin here many a time but never really understood it. Thought it was only for the bottom of the cut! Now I see that it can be along the cut by using a climb offset to improve cut quality then come back with conventional to take off a few thou but without an offset to get better tolerances........I will test this strategy out ......
My history has always been hand and table routing where climb is nearly never used.

Cheers

[gerryv]

Andrew…
Climb and conventional cutting are two very useful tools in our arsenal… Knowing when to use them is critical to success!
As a bit addresses the wood, a tapered chip is removed. A conventional cutting direction removes this chip from the thin to the thick part of the chip, while a climb cut hammers into the wood at the thickest part of the chip, thus the climb cut isn’t quite as smooth as the conventional cut. HOWEVER the conventional cut is more prone to splintering! Some woods like western Cedar will start a splinter and run it the full length of the board! A climb cut will cut these splinter prone grains off, so it can’t run.
How to get the best cut every time…
Almost without fail, you can get the best cut possible in wood using what is called an “onion skin” cutting strategy. This method Uses both climb and conventional cutting to their best advantage. First, make a Climb cut with about a .01 to .015 allowance. This means you have just a little “Onion skin” of material left to remove to get to finished size. Next, repeat the cut in the conventional direction without any allowance. The cut in the conventional direction can be made full depth in a single pass as only an onion skin of material is being removed. This same strategy can be used on the depth as well as the edges… doing it on the depth leaves a continuous tab in place while the most cutting forces are being used.
BTW… cutting in a raster pattern leaves you reversing cut and climb each pass. This can leave you with tear out in the bottom every other pass, making it hard to sand smooth.
SG

Steve,
Is there any need/benefit to using a slight offset for the climb cut so that the final conventional cut will tune up the first cut face - or is that perhaps taken care of by differing deflection (purely a guess)?

[steve_g]

The allowance absorbs any chatter caused by the climb cut pulling machine flex and backlash… IMHO, if you are experiencing any significant amount of bit deflection, you need to rethink your choice of bit and speeds.
SG

[Ajcoholic]

Today I measured a selection of bits from three manufacturers - in 4 sizes.

Across the board, I found the following:

.125 diam bits actual size 0.1235"
.25 diam bits actual size .2455" to .2465"
.375 diam bits actual size .3715"
.5 diam bits actual size 0.4975"

All shanks were from exact size to .0005" under size (half a thousandth under)

so basically the approx 2 to 3.5 thousandths the cutters are undersize would account for the grinding from making the bits from ground carbide stock.

I used a $250 Mitutoyo vernier caliper to measure. Pretty accurate and reads to 4 decimal places.

[Brady Watson]

Few router bit companies can even grind a V-bit to the proper exact angle, so I place little trust in the dimensional integrity of their other 'router bits'...Unless I need an O-flute, v-bit or downcut, I'm using a 2-flute micrograin carbide end mill for cutting.

If you buy a premium tool (not an Ebay special) you can contact the manufacturer rep or reseller if you have a problem with the tools you've been buying. Many times they will replace that tool free of charge and in some cases give you some extras for your trouble. Most shops that are rockin & poppin on a daily basis already have a tooling rep to answer questions like this thread - and many times will visit your shop as a courtesy.

-B

[aschutsky]

Andrew…
Climb and conventional cutting are two very useful tools in our arsenal… Knowing when to use them is critical to success!
As a bit addresses the wood, a tapered chip is removed. A conventional cutting direction removes this chip from the thin to the thick part of the chip, while a climb cut hammers into the wood at the thickest part of the chip, thus the climb cut isn’t quite as smooth as the conventional cut. HOWEVER the conventional cut is more prone to splintering! Some woods like western Cedar will start a splinter and run it the full length of the board! A climb cut will cut these splinter prone grains off, so it can’t run.
How to get the best cut every time…
Almost without fail, you can get the best cut possible in wood using what is called an “onion skin” cutting strategy. This method Uses both climb and conventional cutting to their best advantage. First, make a Climb cut with about a .01 to .015 allowance. This means you have just a little “Onion skin” of material left to remove to get to finished size. Next, repeat the cut in the conventional direction without any allowance. The cut in the conventional direction can be made full depth in a single pass as only an onion skin of material is being removed. This same strategy can be used on the depth as well as the edges… doing it on the depth leaves a continuous tab in place while the most cutting forces are being used.
BTW… cutting in a raster pattern leaves you reversing cut and climb each pass. This can leave you with tear out in the bottom every other pass, making it hard to sand smooth.
SG

Steve - Thanks! I've been doing a bit of reading and should be quite a bit better off now. I do have one question though - How is the 'allowance offset' feature best utilized?

Justin - I've got a few sets of good calipers, but need a nice digital depth gauge. Thanks for the links!


I've been cutting projects for well over a year now, and when you think you know 'enough' you've still got plenty to learn. I love this place. :)

[Kyle Stapleton]

One thing I know, is that I know enough to know that I don't know enough.

[scottp55]

Andrew, If your calipers "Tail" is flush when zeroed out, then just insert tail into hole/groove and read. More accurate when used with an engineers square to hold a true 90. Not quite as good as dedicated, but close enough for most wood work.

[steve_g]

“How is the allowance offset feature best used”…
Andrew:
When I first started designing for CNC cutting, I had to draw the offset vectors for the allowance. With today’s software it’s simply entering a number in a menu box! The same vector can be used for multiple toolpaths with multiple allowances. This sure keeps the drawing simpler/neater.
I pretty much use allowances and onion skin cutting on every cut I do. My toolpath names typically look something like this: “6X6 box perimeter rough” & “ 6X6 box perimeter finish”.
Remember, an allowance can be a negative number as well! When cutting a box joint, I might have an allowance of .010 for my “rough” or climb cut while my finish cut might be -.003”. the negative .003” on both parts will give me a clearance of 6 thousandths (a good place to start to find what clearance todays material/bit/temps/humidity/feed speeds want).
I’m not sure I answered your question, but I’m more than willing to try again if you can point me in a direction!
SG

[shilala]

I asked my brother, who's a machinist, what was up with the undersized mill deal.
I had guessed that undersizing was engineered in, and was acceptable. An oversized mill would never be acceptable for obvious reasons.
He said that in the old days they undersized bits because of the composition of the bits, being that they'd grow under heat. Then as carbide improved, so did the tolerance.
He said the best mills, by Niagara Cutter, in large diameters (2" up) are normally 1-2 thousandths under.
As the mills get smaller, the tolerance gets larger, just by virtue of making the bits, taking into consideration how they'll react under a load.
Another reason the tooling is undersized is to account for chipload in different materials (metals).
"Tool Drag" or friction will literally pull metal along with the sides of the bit, changing the dimension of the cut.
Ideally, taking all things into consideration, a machinist can get perfect or near perfect cuts.
They also used "hogging bits" that we'd call "clearing tools" to remove large amounts of metal. They were commonly 15 thousandths under.

Being as tooling for composites and wood doesn't need such incredible tolerances, and we can "work with it", I'm guessing there's no need to make two different types of bits.
Using dimensions for machinist tooling just makes sense, and keeps cost down rather than making a more accurate cutter for guys doing what we do.

I used to fix all the cooling on the cnc machines at Niagara Cutter in Reynoldsville, Pa, and have watched gazillions of mills being ground.
In order to grind them, there's deflection. The bits are roughed, then they're ground to size and sharpened.
The fact that they are so close is really pretty remarkable.

That's my two cents, and worth about as much. :)

[aschutsky]

“How is the allowance offset feature best used”…
Andrew:
When I first started designing for CNC cutting, I had to draw the offset vectors for the allowance. With today’s software it’s simply entering a number in a menu box! The same vector can be used for multiple toolpaths with multiple allowances. This sure keeps the drawing simpler/neater.
I pretty much use allowances and onion skin cutting on every cut I do. My toolpath names typically look something like this: “6X6 box perimeter rough” & “ 6X6 box perimeter finish”.
Remember, an allowance can be a negative number as well! When cutting a box joint, I might have an allowance of .010 for my “rough” or climb cut while my finish cut might be -.003”. the negative .003” on both parts will give me a clearance of 6 thousandths (a good place to start to find what clearance todays material/bit/temps/humidity/feed speeds want).
I’m not sure I answered your question, but I’m more than willing to try again if you can point me in a direction!
SG

Thanks Steve! Your explanation along with Vectric's forum helped clarify. For anyone else curious, this example helped me to understand:

http://support.vectric.com/aspire-questions/item/what-is-pocket-allowance-used-for

Man, I wish I had seen this feature earlier! So many times I had gone back and modifed/enlarged all my dados when I couldn't just used this. :p

[steve_g]

Andrew…
Your link brought up an interesting point… A pocket allowance Vs a perimeter allowance. A + allowance in a pocket gives a smaller pocket while a + perimeter allowance gives a larger part. The thing to remember is that you are cutting off the line with a + allowance and over the line with a – allowance.
Also interesting to note, a climb cut direction is reversed on an interior cut from what it is with an exterior cut. Vectric software keeps track of this for you if you are using their software…
SG

[David Iannone]

Few router bit companies can even grind a V-bit to the proper exact angle, so I place little trust in the dimensional integrity of their other 'router bits'...Unless I need an O-flute, v-bit or downcut, I'm using a 2-flute micrograin carbide end mill for cutting.

If you buy a premium tool (not an Ebay special) you can contact the manufacturer rep or reseller if you have a problem with the tools you've been buying. Many times they will replace that tool free of charge and in some cases give you some extras for your trouble. Most shops that are rockin & poppin on a daily basis already have a tooling rep to answer questions like this thread - and many times will visit your shop as a courtesy.

-B


I agree.

I have been using (and breaking) $40 Onsrud bits for years.

Just recently bought some bits from ebay (drillman1) and am happy with some of them. You get what you pay for yes.....you just have to know when to hold em, know when to fold em.....etc

Dave