pocket toolpath not even

[rseeley13]

I was making a tray and when I pocket out the tray area the pocket path does not match up with the pocket clear path. (I am using a 3/4" core bit to do the pocket and a 1/2" end mill to do the pocket clear) As you can see in the photo there is a little ridge that is left between the two and is a pain to sand out. I am zeroing both bits in the same area each time. Any suggestions?

[Brady Watson]

Is it possible that the core bit is off a little on one side compared to the other? If you bring it down close to the work/plate, does one side of the split tip look like it will contact before the other? I've had some where one side touches and the other doesn't. They aren't made with precision in mind...

If you can repeat the problem, then just modify your final depth up or down in the toolpath until you get a smooth transition between the two. Only .005-.01" increments until you sneak up on it & it goes away.

-B

[scottp55]

Had the same problem awhile back(see thread).
Did you Z-zero second bit in the exact same spot on the wood and your plate as you did on your clearance tool?
Yep, a bear to sand if you take it off the machine too soon.
Got some good advise Here.
http://www.talkshopbot.com/forum/showthread.php?t=19075

[dlcw]

I did notice, in your picture, some ridges where your core bit cut. It looks like either what Brady said about the bit not being symmetrical or the spindle is not perfectly perpendicular to the table in all directions. This could contribute a little but not as much as what your picture is showing.

I've had this problem in the past using Onsrud bit (higher quality). Making sure my spindle was perfectly perpendicular helped eliminate some but not all.

The only thing I could attribute it to was when I hogged out the board, its dimensions changed (stress release in the wood). When I z-zeroed in exactly the same spot, it didn't matter because the change in the board caused the z-zero to not be the same. The preview in Aspire showed everything good to go. Ended up sanding it out.

[rseeley13]

Does anyone have any suggestions on a better way to make pocketed trays?

[rseeley13]

How do you adjust just the clearing toolpath in the pocketing toolpath? I only see the depth on top that can be adjusted and not the larger bit clearing.

[Brady Watson]

You could clear out with a single tool (making sure to offset vector inwards so you don't eat into the cove) - and then do an inside profile cut with the core box using your original vector, adjusting the depth as needed on either toolpath.

Some jobs require an out of the box approach and little tweaks to get you where you need to be. It seems odd, but that's a day in the life of a machinist.

-B

[bleeth]

Guy's:
Here is the bottom line of what i have learned over the years when it comes to zeroing different bits when using a Shopbot. When using the zero plate different bits will zero at very slightly different heights than other bits. This will result in ridges in some toolpath strategies.
Weirdly, it also happens when using the same bit zeroed only once with some 3-d toolpaths. Frankly, I believe it is an inherent issue that is unsolvable in any PRODUCTION oriented project that don't really allow you to cut a variety of experimental samples until you hit on the final excruciating and high time consuming method that gets the different bits to meld the results together properly when setting them up with the built in z zeroing system in a time efficient manner.
The PRS Alphas, when doing a 3-d file with a single bit, result in a better resolution result than older or lesser advanced SB's, but they all have that issue.
I have never seen a 3-d project come off a SB, or in fact any CNC that didn't cost a huge amount of money, that didn't then need a considerable amount of sanding to really make it high-end sweet. It is what it is.
I have been told that some machines that are fully welded, balanced, and milled, and also run from servos, linear rails, and ball screws are more accurate. I have no reason to doubt the folks who have told me this. They also admit that those tools cost them a heck of a lot more than the average SB.
(Just one of those days when hearing about how tough it is to get a SB to cut everything perfect without some actual physical work afterwards to clean it up is too repetitive)

[rseeley13]

Thanks for the info, I will give it a try. Just thought that I would be able to do this in the pocket toolpath function.

[srwtlc]

Ryan,

Try a good quality bowl & tray bit. I use the 1.25" diameter ones for production work and can easily sand out any marks. Best ones I've had are CMT, Jesada, and Infinity. Cheap ones can sometimes not be flat across the bottom.

[scottp55]

Thanks for chiming in Scott, Was going to reply,but never bought the Infinity and my SETools 3/4" (with the extra brazing removed that caused lines)still isn't perfect. Best/easiest finish for me up to now on smaller pocket is a .5"BallNose and hogging out with a .02" pocket allowance and a 49-50% stepover climb cut, Then a full depth skin pass with a ramped lead-in profile pass first conventional cut with feed/speed increased, BUT the 5-8% stepover needed for minimal sanding is a dealbreaker for production times.
Thanks for the extra 2 suppliers-Got to get one of them Puppies:)(probably only a 1" for the Desktop though).

[Brady Watson]

I have never seen a 3-d project come off a SB, or in fact any CNC that didn't cost a huge amount of money, that didn't then need a considerable amount of sanding to really make it high-end sweet. It is what it is.

That sounds so negative about SBs and not true. If you are a noob @ 3D - yeah OK, but that is true on any machine. Visit my shop...I'll show you how it's done on my 14 yr old PRT first, then on my Desktop machine. All carvings require at least some sanding - not to correct blems or erase tool marks, but to prepare it for finishing - no matter what color the machine is.

-B

[scottp55]

Brady, Off topic slightly, but just started noticing when VInlaying that I could run the male pass 4 times(I was working on something else at the time so just kept RR'ing to get the VERY last fuzz off) and had the vac off and even after 3 passes I could STILL hear it cutting an infinitesimal amount. True that was probably wood movement on the 1/4" stock, But to some extant it even happens on 6/4.
NOT enough to worry about at ALL, but just about to go into shop to do the Z-Mod on the Desktop and wondering if there is anything special to look for while I've got all ripped apart?
Now I'm going to regret Razzing you yesterday! I just KNOW it!!:)
Grateful Acolyte

[Brady Watson]

NOT enough to worry about at ALL, but just about to go into shop to do the Z-Mod on the Desktop and wondering if there is anything special to look for while I've got all ripped apart?

Scott,
No worries.

How did you tram the Z when you put it on? I use the tail of a digital caliper to check spindle to spindle plate parallel and then use a dial indicator against the spindle mounting plate and run it up & down to see if/where it is out - then adjust accordingly. It's a little time consuming - but it's one of those things that will shoot you in the foot until you get it *perfect*.

A word to the wise - for anyone doing the longer Z - put a dab of Never-Seize on the Z to spindle mounting plate or they will lock up on you. I had to grind a slot in 2 of mine & then impact them out with a screwdriver & hammer. Galvanic action of steel to aluminum is rough...

-B

[Burkhardt]

........started noticing when VInlaying that I could run the male pass 4 times(I was working on something else at the time so just kept RR'ing to get the VERY last fuzz off) and had the vac off and even after 3 passes I could STILL hear it cutting an infinitesimal amount.....

Besides the possible wood movement keep in mind that depending on your milling direction (conv/climb) the bit is pulled left or right relative to the machining direction. The amount depends on the bit flex (a slim end mill or a v-bit with 1/4" shank will be less rigid than 1/2" shank). The fact that the very tip of a sharp v-bit does not actually cut but only drags through the wood probably does not help. On top of that you have spindle/router bearing play and machine flex, although I would guess the Desktop is pretty rigid. Therefore the second cut will usually still remove substantial material. Doing further cuts on my machine I still can hear sometimes but I see no chips or dust so I guess the flutes just touch protruding wood fibers, making that whirr.

[scottp55]

Thanks Brady/G.
Unfortunately Brady, I got to read it after I was all finished as trying to get my helper back to HIS shop.
Good info! Can I copy/paste onto Z-Mod Thread?
Forgot about Galvanic but did Boeshield both plates and wiped off excess and used same rag to wipe back of spindle. Didn't Tail anything, but my Iron Age $1.69 Ace Hardware 1/8"X12" (.1238") brass rod from hobby section made a decent(for me) trammel. Used Starrett 12" rule from my square laid flat, got close, and Fixed moved down .01" at a time and got it pretty close.
Interesting was Fixed Move was abrupt enough to cause visible oscillation at the tip(9" away from spindle center). Then I set Fixed Mode to .005" and got all 4 points of the compass to where a fixed move up let it vibrate, and then a Fixed Move down dampened it.
Close enough and done for today.
Thanks again, and sorry to get off topic. Will post on Z-Mod thread.

[rseeley13]

Ryan,

Try a good quality bowl & tray bit. I use the 1.25" diameter ones for production work and can easily sand out any marks. Best ones I've had are CMT, Jesada, and Infinity. Cheap ones can sometimes not be flat across the bottom.

Scott,
I would have used that but this design has curves that I couldn't fit a large bit in the corners. Had to use a smaller core bit and then an end mill to clear out.

[srwtlc]

They make a 3/4" one, but I haven't gotten as clean/smooth results with them as the larger ones.

[Kyle Stapleton]

I thought you were on vacation?

[srwtlc]

I am.....gotta check in when we hit the next hotel/WiFi ya know. :)

[scottp55]

Scott, Curious what kind of pass depth you use on that 1.25" Bowl/Tray if you are indeed "hogging" with it when you get back from Vacation. Enjoy!
Wondering "So where IS a Wisconsinite when he's not at Home?" :)

[chiloquinruss]

If you've followed any of my 'juniper' posts you know how much I love the look but hate the wood! :rolleyes: Anyhow what I have been doing is hogging out the material and letting it set for a bit (an hour or so) and this gives it some small amount of time to do whatever it is going to do. Then I re-z-zero to the new bottom and make a finish pass using the new setting. Works for me but only if the it is the wood that is misbehaving and not something on the machine. Large hog outs like bowls and such require an absolutely perpendicular Z. Russ

[srwtlc]

Hey Scott,

Depending on what I'm doing and how deep the finished depth is, I'll go either 0.125" or 0.25" per pass, 3-6 in/sec @ 10k-14k. These are non-plunging bits, so they must be ramped into the cut.


Wondering "So where IS a Wisconsinite when he's not at Home?

Well, this couple made a big loop (across the top on the 'Highline') to Glacier National Park, Yellowstone, The Big Horns, Devils Tower, Spearfish Canyon, Needles Hwy, Custer Park, Jewel Cave, Mount Rushmore, and the Bad Lands. ;)

[scottp55]

Thanks Scott, Going to have to pick one up(too bad 3/4" doesn't do as good a job).
Sounds like a beautiful vacation, also sounds like one of those where it's nice to get home:)
scott

[chiloquinruss]

Scott W. you missed one in that same area, Crazy Horse! Best museum on our cross country trip! Glad you had a great time, we loved that whole experience. Russ

[srwtlc]

Oh yeah, went past it twice as we went back and forth to our hotel in Custer (didn't go in though). Recommended roads if you're ever in any of these areas....Going to the sun road, Blackfoot scenic byway, Chief Joseph scenic byway, highways 14 and/or 16 over the Big Horns, Spearfish Canyon road, Needles highway, and Iron Mountain road. Lots of oohs & aahs and plenty of pucker factor for the person on the down side of the road! :)

Scott, my first 3/4 one seemed to work fine at first, but I think one of the resharpenings got the bottom plane out of true. If these kind of bits aren't flat across the bottom, it will take a lot of sanding to get the marks out. I have two Jesada 1.25" ones that have been resharpened to the point that they can't be again and they still cut great. I have one cheap brand one that I used once and it is now only used for filleting on the router table.