"nicks" in female inlay machining

[bking1836]

Hi all,

Today's inlay production work went a little wonky, and I am curious if anyone has any insight. You can see clearly that it was cut in two passes, which is the minor issue. The bigger issue is the strange "nicks" that were consistently in the same places.

32225

I used VCarve Pro's female inlay toolpath like I always do. Only difference was I used a new type/brand of 1/8" downcutter. The male inlays using the same bit came out fine. And the large area clearance part of the toolpath went fine too.

Thanks for your help!
Brian

[EricSchimel]

Is it possible you lost some steps there? It looks like the tooplath got shifted...

[Brady Watson]

Machine model? Cutting speed? RPM?

If PRS gantry tool - Wiggle the YZ car in ALL directions with the control box on. Feel slop? Tighten lower V-roller bearings. Wiggle Y+/-, slop? Reseat pinion to rack. Wiggle EACH X motor side front & back. Sloppy? Reseat pinion to rack...

DT/Max/PRT/PRS Standard? Slow down...

[bking1836]

Is it possible you lost some steps there? It looks like the tooplath got shifted...



Machine model? Cutting speed? RPM?

If PRS gantry tool - Wiggle the YZ car in ALL directions with the control box on. Feel slop? Tighten lower V-roller bearings. Wiggle Y+/-, slop? Reseat pinion to rack. Wiggle EACH X motor side front & back. Sloppy? Reseat pinion to rack...

DT/Max/PRT/PRS Standard? Slow down...

It's a PRS Standard. 13500 rpm, 3ips, 2ips plunge, 1/8" downcutter on hard maple. 1/8" passes.

This happened consistently across 12 of the same inlays (they are cheese boards with wine glass inlays). And this morning I realized that the wonky parts are all where the bit plunges and retracts, which has to be significant, right?

I will check that everything is secure this morning.

[srwtlc]

Bit deflection. How long is the tool? Cutting edge length? Sharpness? Ramp your plunges. Try a shorter tool. I really like using the 1/8" shank, 1/2" CEL, 1-1/2 long ones from here (https://www.ebay.com/str/CARBIDE-PLUS?_trksid=p2047675.l2563).

[bking1836]

Bit deflection. How long is the tool? Cutting edge length? Sharpness? Ramp your plunges. Try a shorter tool. I really like using the 1/8" shank, 1/2" CEL, 1-1/2 long ones from here (https://www.ebay.com/str/CARBIDE-PLUS?_trksid=p2047675.l2563).

The irony is that it's a brand new tool, and shorter than what I normally use (1/2" CEL vs 3/4"). I ramp the plunges always. Get them from these guys in Oregon and have been very pleased with their 3/4" CEL 1/8" bits. https://www.ebay.com/itm/1-8-Solid-Carbide-DownCut-Down-Shear-Router-1-2-Cut-2-Flute-Square-USA-5-Pack/253873726413?ssPageName=STRK%3AMEBIDX%3AIT&_trksid=p2060353.m2749.l2649

[EricSchimel]

There's no way that's bit deflection... From the looks of it that is about a 1/16th or more that the path is off. If you put a bit in a vice and tried deflecting it that much with pliers it'd snap long before it got that far off. Assuming the machine is tight, something else is going on here...

It looks to me like the whole toolpath is shifted up towards the top of the screen (Y direction?) Based on your previous static woes, my guess, and it's just a guess, is that you've lost some steps here. You can see it on the top left of the image too...

[bking1836]

Here’s a video of the slight slop in the YZ car. Similar amount on the control box side X motor. Other side X motor seems tight. I’m not sure what/how to tighten.


https://youtu.be/KKYQjmcGk4k

[bking1836]

It looks to me like the whole toolpath is shifted up towards the top of the screen (Y direction?) Based on your previous static woes, my guess, and it's just a guess, is that you've lost some steps here. You can see it on the top left of the image too...

But it happened essentially the same on 12 separate pieces all part of the same cut.

See video in post above for the slop I’m experiencing. And isn’t it relevant that it’s happening where the bit plunges and retracts?

Here’s a different inlay on the same job. 32226

[srwtlc]

That's way too much slop! Check that pinion for tightness to the shaft and engagement into the rack. How worn are the pinions? As for the toolpath, you can make the profile pass first to keep the tool from being side loaded when it moves out for the profile. I prefer longer smooth ramps to zig zag. A smooth ramp will also relieve the bit as it finishes the cut before lifting.

[bking1836]

Machine is 1 year old and has gotten decent use but certainly not all day every day production work.

Rack and pinion on YZ car:
32227

Rack and pinion on control box side at X motor:
32228

[srwtlc]

Looks a little worn and mis-aligned on the YZ as well. Kind of dry too! I'd get some new ones and some good lube too.

[bking1836]

Detached and reattached all the stepper motors and things are tight now. I have another 16 trays to make and I’ll be able to compare the difference.

FYI Fanowood latex wood filler is amazing stuff to hide the imperfections.

32229

[Brady Watson]

ALL machines need maintenance. Follow the assembly guide available under the Support area on the main SB page. Observe how things go together and make them right.

You're machining entirely too fast for that machine. You are losing steps or the machine is deflecting. The part you show appears to be less than 4 or 5" wide. There isn't enough room for the tool to accel to 3 IPS and Decel to 0 IPS in that distance...that means you're not running at a properly set speed to start with. Furthermore, small tools NEED high RPM to at the very least get into the right chipload range. You should be running that 1/8" around 18,000 RPM and your MS somewhere in the 1.5 to 2 IPS range.

When quality sucks, slow down AND check your machine...but you should already be doing that regularly in addition to CLEANING the machine regularly...RIGHT? It needs more attention & maintenance than your other woodworking power equipment.

Question for EVERYONE: Have you ever seen a solid carbide tool deflect? I never have. Carbide is crystalline in composition and will SHATTER and snap off before it ever deflects. High Speed Steel (HSS) WILL deflect. Carbide = Nope. QUESTION #2: If the bit isn't deflecting, then what is? Follow the line of logic and find out what needs to be adjusted or if you are machining too fast.

Bonus - If you are using speeds straight out of the default tool database in the Vectric products, stop immediately. There was no logic behind the numbers that programmers put in there as sample data...you NEED to pick the right speeds for the work YOU are doing.

[bking1836]

ALL machines need maintenance. Follow the assembly guide available under the Support area on the main SB page. Observe how things go together and make them right.

You're machining entirely too fast for that machine. You are losing steps or the machine is deflecting. The part you show appears to be less than 4 or 5" wide. There isn't enough room for the tool to accel to 3 IPS and Decel to 0 IPS in that distance...that means you're not running at a properly set speed to start with. Furthermore, small tools NEED high RPM to at the very least get into the right chipload range. You should be running that 1/8" around 18,000 RPM and your MS somewhere in the 1.5 to 2 IPS range.

When quality sucks, slow down AND check your machine...but you should already be doing that regularly in addition to CLEANING the machine regularly...RIGHT? It needs more attention & maintenance than your other woodworking power equipment.

Question for EVERYONE: Have you ever seen a solid carbide tool deflect? I never have. Carbide is crystalline in composition and will SHATTER and snap off before it ever deflects. High Speed Steel (HSS) WILL deflect. Carbide = Nope. QUESTION #2: If the bit isn't deflecting, then what is? Follow the line of logic and find out what needs to be adjusted or if you are machining too fast.

Bonus - If you are using speeds straight out of the default tool database in the Vectric products, stop immediately. There was no logic behind the numbers that programmers put in there as sample data...you NEED to pick the right speeds for the work YOU are doing.

Thank you Brady. You are, as ever, and invaluable resource. I will adjust feeds and speeds per your advice. Makes sense now that I think about it. I am only a year into this whole CNC thing, so I am still on the steep part of the learning curve for sure. Getting there.

I had already taken the opportunity to clean and lube up the machine. I was certainly behind on that.

[paul_z]

This is a bit off subject but might surprise a lot of people. Carbide bits are not solid carbide. If they were, they'd be extremely expensive and brittle to the point of being useless.

“Cemented tungsten carbide,” the material that makes up the tools and inserts, is actually grains of tungsten carbide, along with particles of other materials, cemented together using the metal cobalt as a binder.

Tungsten carbide is actually a good electrical insulator (if my failing memory serves me). Why then can you use an electrical ZZero plate? Metallic cobalt is a very good electrical conductor.

Even though the bit is not solid carbide, it is extremely rigid and flexes very, very little before breaking.

Paul Z

[EricSchimel]

Brian.. I totally missed that video... You've got to correct that slop. As others have said.. go back through the setup instructions and tighten the machine up. Looks like you've got some V rollers that aren't adjusted. What's not obvious is that the V rollers are excentric and can be tightened with an Allen wrenches and a flat wrench (I use one for a mountain bike)

[a.werby]

It's made by sintering grains of tungsten carbide with cobalt metal, which produces a solid material that's ground to form tools. The endmills referred to earlier in this thread are sold as "solid carbide", not to be deceptive, but to differentiate them from router bits that often are made primarily from steel, with carbide cutting edges brazed on.

[Brady Watson]

A bit of thread drift regarding carbide...

Yes, 'solid' carbide within the realm of tooling is most certainly 'glued' together. The term 'micro-grain carbide' is of interest, because an endmill is essentially constructed of very tiny balls/spheres of carbide (and other 'stuff'). Just like changing the resolution in your favorite Vectric software to alter the size of the 3D pixels, or voxels - carbide grain size is along the same lines. Think of micrograin as higher resolution...well, sorta.

But why does it matter what size the carbide grain is - to me, a CNC router guy?

It matters because carbide HATES heat. When carbide is overheated, it readily ejects from the surface of the tool and never goes back...that means that if you were to observe this happening, there would be a series of 'pock marks' out of the cutting edge of your tool that migrated away from the tool because it was overheated. Imagine if you will that the tool you are using was a cheap import - the grain size would be quite large compared to a premium micrograin carbide tool. When overheated, more carbide leaves the tool volumetrically than a micrograin one...So, more of your cutting edge goes bye-bye as a result.

This is why it is recommended that you cut CHIPS and not make dust with your cutting, because those large chips act as a heat sink and carry the heat away from the tool - saving your cutting edge and your carbide. There are coatings available to insulate the carbide from heat, but you should know - NO coating has been proven to be advantageous for CNC routing of wood because it just doesn't get hot enough for the coatings to be effective...So gold colored tools that promise to last for eternity when routing wood should be relinquished to the snake oil pile...The exception here, as it relates to routing (if you call your CNC router a mill, I'll slap you...) - is diamond coating. This gives zero heat resistance, BUT offers increased hardness @ the cutting edge, which can be a real advantage with composites...and there are a number of different types of diamonds too...and none are cheap, but they ARE worth it if you need them.

When it comes to micrograin carbide, it is possible to achieve a sharper edged tool, compared to a coarser grain carbide tool. However, if you do some research on the subject of cutting tools and the materials they are made from, you may discover that other materials, such as high speed steel (HSS) and other materials are much SHARPER than carbide when comparing identical grinds. This is because the molecules are smaller, allowing it to hold a sharper edge. However, HSS is much softer on the hardness scale & 'hardness' means the resistance to scratching...so an HSS tool might be sharper, but can't hold its edge as well as a carbide one.

Those cutting aluminum might want to try HSS. It is 'tougher' than carbide because it will deflect a little - BUT, it also absorbs harmonics when cutting AL and can give better results. It is certainly worth a try...and YES, they are sharper, so don't slice your finger sliding down the helix...like I did...a few times...:p

[jerry_stanek]

Yes I have seen a .125 bow just a little and not break

[srwtlc]

(if you call your CNC router a mill, I'll slap you...)

.........:D