Multi-cam tool marks

I’m trying to cut pretty thin profiles on the multicam. I was able to get the pieces cut out using a spiral ramp move but the bit leaves pretty deep tool marks following the spiral path that are pretty hard to sand out (See pic)

I’m cutting pine using a 3/8" downcut endmill (1/4" is too short to go all the way through material) with the database feed and speed settings for softwood. I have the passes set to 8 to cut through roughly 1.5" thick material. All my settings are in the second pic

I really appreciate any advice.

image

​​​​​​​​​​​​​​​​​
Why?

It’s what I used during my training; I’m not extremely knowledgeable about CNC yet.

First things first the material you’ve chosen (pine?) doesn’t have a very dense, consistent structure so the end grain is going to be pretty friable.

Second thing is it looks like the cutter might not be cutting on the outside edge leaving a little bit of each pass standing to be torn out when it comes back again. Is this a Makerspace endmill that might have a chip out of it or even just a dull cutting edge? I’d recommend getting your own set of endmills to bring into the space.

Also a down-cutting endmill is usually used when you need to make sure a thin material is not going to come off the table; they are also useful when you need the top edge to be perfect (not the top surface). If you imagine cutting along side the edge of a board the fibers can either be torn up out of the board where they can peel and get tearout or they can be cut by shearing them downwards against the rest of the material like a pair of scissors.

The last thing is that I think I saw a thread a week ago or so that said that the head needed to be trammed (made perfectly perpendicular with the table). If you imagine the cutter being tipped slightly as it cuts it would cut deeper on one side and shallower on the opposite. Not sure whether this could be a big enough factor to get this effect.

3 Likes

Thanks for the advice. I was cutting out of pine because I wanted to practice on a cheap wood before trying with something fancier (and more expensive). This is a makerspace endmill; I’ve got no problem buying some bits of my own. I would like the top edge to be good quality, so maybe a first pass with a downcut followed by the remainder with an upcut?

I would try starting with an uncut for the whole program and if you don’t like the edge add the downcut step. Another tactic if you are going to be surfacing the top anyway (which it looks like you were doing in the sample) is to cut the edge first w/tabs and then let the surfacing remove any imperfections.

Surfacing end grain can be difficult to get a nice surface finish because the fibers like to bend over in the direction of the swirl like the grass with a lawnmower. The best strategy I’ve seen (not exhaustive by any stretch) is to cut every pass in the same direction and use a lot of sandpaper.

Just adding that running test cuts on poplar from Central hardwoods tends to be a cheaper solution and is more stable than pine.

4 Likes

I can’t tell if it’s the case here, but I’ve found the database speeds/feeds to be much too fast. I generally buy and use Amana bits and their recommended feed for a 3/8” 2-flute carbide downcut bit is 210-290 IPM.

Our feeds were very high for 1/8” bits and I got much better cut quality (my primary issue was chipout) after dialing back the the manufacturer recommended feed rate.

You might also try a final full depth (one pass) climb cut along that profile to see if it cleans things up a bit. AFTER cutting the profile with your other incremental cuts.

2 Likes

Is the end mull fully engaged? (stock on both sides; you’re cutting a slot around the part)

A downcut is the correct bit, especially on pine.

Just looking at it, the pictures perspective makes it hard to visualize the cut. Is is a circular radiused cut, and you’re trying to round off the top edge on your way to the bottom? If so, on a part that small, a big bit is going to leave lines like that. If you need a fine finish, rough it out with the 3/8, then switch to a 1/4 or 1/8 ballnose, and set the stepsize way down. It’ll take a while, but thats how you get a nice radius on rough sappy wood. On the 3/8, you can do vertical stepsizing by reducing the depth of cut down to about a tenth of the bit diameter. It will still be rough, but maybe not quite as rough. 3/8 bits are for hogging out lots of wood fast. Not finishing bits.

2 Likes

No idea what they are now, and may have been changed. But the tool library I left in it, was done by calculating the chipload for each of our stock bits. There is one, and only one correct F&S ratio for any given bit/cut depth, and that’s the one that runs at the correct chipload for the bit. Any other speed, is either damaging the work, or damaging the bit. Physics is physics.

Every CNC router user should know how to calculate the chipload/F&S for a given bit, bring in their own (sharp) bits, and the tune the F&S to reflect the type of wood, and depth of cut/finish desired. The formulas are well known, and simple arithmetic. If you’re getting crappy results, accept it as a learning experience - it means you suck, so read more, ask more questions, and soon you’ll be whacking out the sweet stuff.

When I was maintaining the machine, we threw away an awful lot of bits, ruined by people slowing them down, causing them to overheat, lose temper, and stop cutting. The process of evacuating chips from the bit, is the primary means heat is removed, and when you stop making chips, and start making dust (because slow), you’re ruining a bit, sure as shooting.

Easy check - cut three or four inches with the bit at your proposed speed in the spoil somewhere. Look at the sawdust - is it dusty or glazed, or blackened? You were too slow. Is it the texture of meal? Hey - good job operator. Is the bit hot? If it is, you were running too slow, and possibly ruined the bit. Calculate the chipload F&S, and use that. Notice the bit cuts faster and cleaner, and isn’t hot at all? That what happens at chipload.

I guess I assumed that this was a flat surfacing cut but it could be a profile cut. Can’t really tell from the image.
I definitely don’t think that its a cut that requires a ballnose though. It doesn’t look like there is any intended contouring to do.

Edit: and if I just read it properly the first time I would have seen it’s a spiral profile cut.:roll_eyes:

Lol. I suck? Ok.

I did calculate the chip load. For my bits. And using those feeds/speeds went swimmingly.

Looking at the 1/8” upcut in soft plywood, our VCarve database f/s is [email protected] That’s for the Onsrud 52-240. That is insanity.

Referring to the Onsrud data for that bit, which is a 2-flute, the recommended chip load per tooth is .005-.007” for hard/soft plywood. At 18k rpm, that’s 180-252 ipm NOT 324.

I did, and what I learned is to not trust the feeds/speeds in our tool database, which can’t be changed (and then saved) by users. It isn’t accurate for DMS bits, much less similar bits brought in from home.

Maybe this is why we were burning through bits so quickly.

All inconvenient given that VCarve doesn’t have a reasonable what to simply open (as opposed to import) a custom tool database. I’m going to suggest this to them as a feature.

2 Likes

And approved for use on the jointer; thanks for the tip!

Yes, cutting a slot around the part

1 Like

Here is an extra picture hopefully to clarify. The tool marks I’m complaining about are on the outside diameter

image

1 Like

Yeah, that sounds high. Suspect a “helper” got at the toollib file :slight_smile:

You do want to keep that bit moving smartly in pine, and use a sharp one as well, or your finish is gonna suck. Sap does not help the cut expel heat, and it tends to rebind the chips causing weird and sometimes spectacular blowout.

Yessir. On the nose. Its just a consequence of a lot of new and unfamiliar users using the machine, and it really can’t be helped, though many (including me) have tried. That’s one reason we always advise people to bring their own bits.

Yep. Every person getting past the beginner stage wants the same thing, and that includes me. But vCarve doesn’t really have a great multiuser solution, and if you import your file, the next guy starts there, and might use your settings, whether you knew how to set F&S or not - adding a whole bunch of new steps to the “walk up and use it” regimen that is already a bit busy for beginners to handle. If they would just store a toollib.tapper or toollib.mdredmond in the users windows profile, it would be a snap. Copy in your latest file, and vCarve picks it up and uses it in place of the master toollib. But no.

1 Like

Gotcha. So, if you turn the bowl mouth down, and consider the direction the bit has to move for the circular cut, yoiu’ll see why a big bit leaves steps behind on very steep angles like that. Cuts a ring DOC deep, moves out stepsize, cuts another ring, moves out stepsize, cuts another ring, and so on. So you would expect the surface to be ringed from top to bottom of cut.

Realistically speaking, your stock depth is forcing the big fat long bit, and you’re going to get a rough surface finish regardless of what you do on the machine. The result is just the wood’s way of telling you that shapes like this need to be turned. Lathe mo betta!

1 Like

The Spindle tram should be within a few thousandths of an inch unless the spindle loosened recently. I’m betting its bit deflection.

As I already replied to his PM, doing a 0.005-0.010" larger offset, then a separate finishing pass at full depth at desired offset to clean the edge would help. You can use a strait edge as a finishing bit I’m sure (Onsrud has fancy finishing bits I’m sure for some $$$).

1 Like

He’s using a cut on a profile toolpath to approximate a 3D surface with a 2D tool path. It can be done, but using an end mill always guarantees a stepped surface with each step having an X displacement equal to the step size, and a Y displacement = the depth of cut. All the way down the curve. And end mill will cut with the corner, a ball mill will cut in its anled side, and make steps with no vertex, simulating a smoother surface better.

The right way to do it, is with a 3D model, and 3D tool paths, which can profile vertically far better.- but even then, there’s always some unwanted cutting artifacts. Everything needs sanding, it’s really a question of how much?