Need advise

This forum is for general discussion regarding VCarve Pro
Post Reply
denisddion@gmail.com
Posts: 5
Joined: Thu Oct 24, 2019 4:13 pm
Model of CNC Machine: Axiom I2R

Need advise

Post by denisddion@gmail.com »

I am new to CNC and I have purchased some of the projects from Design & Make. I would like to know if these designs offer any suggestions on which tools to use to cut the project and second it seems like when I check to see the machining time to do the design it's telling me 50 hours or so.,
Is this normal or am I doing something wrong?

User avatar
gkas
Vectric Wizard
Posts: 715
Joined: Sun Jan 01, 2017 3:39 am
Model of CNC Machine: Aspire, Axiom AR8 Pro+, Axiom 4.2W Laser
Location: Southern California

Re: Need advise

Post by gkas »

We need a little more info. Since it's a D&M project you can't post the crv file. How about project size, bits, feeds & speeds? Also, it's OK to post the project preview jpg.

Bob Reda
Vectric Wizard
Posts: 743
Joined: Wed Aug 16, 2006 7:34 pm
Model of CNC Machine: shopbot 48x48 upgraded prt
Location: Monessen, Pa
Contact:

Re: Need advise

Post by Bob Reda »

Depending on the size you are making it, you usually have a rough in pass and then a finish pass. These passes for the most part are done with ball nose bits, for the rough in pass usually a 1/4" ballnose at a step over around 40% will suffice, but then again, you can go bigger if there is not a lot of detail or you are making it a large project. The finish pass is usually a 1/8" ball nose at 10% stepover with the same conditions as the rough in. Your time is dependent on a lot of things, one is size, the other is how fast you have the "z" axis going. In 3d the machine will only go as fast as the z axis. You will hear this a lot but do spend some time with the tutorials for 3d cutting, this will answer a lot of your questions.

Bob

User avatar
Xxray
Vectric Wizard
Posts: 2114
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: Need advise

Post by Xxray »

Just too add a bit, for finish you may need to go far smaller than 1/8 depending on size of the job and detail you want to achieve, I use a bit as small as 1/32. They are costly but you really can't get great detail without them, unless the project is very large. But then, you may need a 1/16, so all of these bits you are going to have to have in your toolkit for optimal results in 3d.

Quite a few sources, including amazon and ebay for cheaper [and generally inferior] bits, this is my go to source https://www.precisebits.com/products/ca ... p&filter=7

As far as projected cutting time, don't worry about it, I believe it needs to be calibrated or scaled to your particular machine before it gives results anything close to accurate. I've never paid much attention to it. Though occasionally there are things you can do to speed up cutting time outside of the obvious step of max IPM, it generally is what it is when it comes to 3D. Especially using the smaller bits I mentioned combined with a low stepover [both necessary for detail], some projects take quite a bit of time, though 50 hours would be epic and not typical.

Most projects say 8x10" or so you should be in the 2-4 hours range, goes up from there with size and complexity.
Doug

User avatar
dealguy11
Vectric Wizard
Posts: 1513
Joined: Tue Sep 22, 2009 9:52 pm
Model of CNC Machine: Anderson Selexx 510
Location: Henryville, PA
Contact:

Re: Need advise

Post by dealguy11 »

For what it's worth, the Design & Carve projects were mostly designed to be cut with a 1/8" ballnose. You can go smaller if you like. Realistically, unless someone will be looking at the carving very closely, go with the largest bit you can get away with. It's hard to tell the difference from a few feet away.

As far as roughing, I almost always do it with some kind of end mill (not ball nose) and use z-level roughing. I don't find that using ballnose bits for roughing really makes a lot of difference. The point is just to hog out as much material as minimally necessary as fast as possible so the finish bit doesn't break. Just make sure the end mill is small enough so that there are no really deep uncleared holes for the finish bit to plunge into.

For finish carving, I use tapered ballnose bits, which can be surprisingly strong. I generally use 1/8". Occasionally I'll go to 1/16" if the work really demands it. I have a 1/32" bit but haven't touched it in years. I have an industrial machine and run my 1/8" bits very fast when carving. I won't say how fast because it's not something that makes sense for most hobby machines. In reality you can't really get faster than about 200 ipm if there is a lot of vertical movement (the acceleration of the machine will automatically slow things down), but on flats the bit is removing so little material that it can easily go a surprising speed without breaking the bit.
Steve Godding
D&S Artistic Woodworking http://www.dsartisticwood.com

User avatar
Xxray
Vectric Wizard
Posts: 2114
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: Need advise

Post by Xxray »

Interesting, I am the opposite, haven't touched my 1/8 tbn in years, guess it depends on size, detail and complexity of the model.

I do know this - OP, always run a preview on your toolpaths, if it looks messed up/not right in preview, the actual cut is not going to be right either. With a larger bit there are often areas in a model, sometimes lots of areas, that the bit cannot get to because of its size. In that case, step down to a smaller bit, recalculate toolpaths then clear and rerun the preview and see if its up to snuff. Ideally, as stated, you want to use the largest bit you can without sacrificing detail.

Just a quick example for perspective - If you were just carving a large dome, it is 3D but really no detail, no crevices, so you could use a large finish bit. On the other hand, if you were carving a model of the last supper same general size as the dome with the same bit, it would look atrocious, so you'd need to step down a size or 2.

Stepover setting [which is a software setting that you set yourself in bit properties] is another factor that determines time of cut vs detail. Lower stepover = higher detail and longer cut times. There is a point of diminishing returns [assuming you are willing to sacrifice time for detail, as most people do] where you may lower the stepover even further and notice no difference in detail. This sweet spot takes experimentation and experience to determine, I usually like to go 12-13% for 3D finish, would not recommend higher than 15% [and yes, even 1% higher or lower can have noticeable results on both cutting time and detail].

Why not just cut through the chase then and set it to the lowest possible, 1% ? Because, as stated above, you would only be drastically increasing cut time with no appreciable benefits to the models level of detail.
Doug

User avatar
TReischl
Vectric Wizard
Posts: 3362
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Need advise

Post by TReischl »

Agree with the use of tapered ball nose bits and the fact that they are much stronger.

Quality of bits is a discussion in and of itself. Frankly, I see little difference between the el cheapo bits and the pricey ones. I push mine pretty hard, program target feed is usually 250 IPM and yup, they get going that fast on the flats or areas with gentle curvature. I have yet to break a bit due to feedrate. Break them because of a dumb move on my part, you bet.

I do some small stuff that demands really tiny bits, like the .25mm (.0098) type. I bought a pack of ten for like $10, they are .125 shank. I have run them a lot including in aluminum and have yet to wear one out. Those bits rarely get above about 40IPM because of the size and detail of the parts they cut.

As DealGuy alluded to, a lot has to do with your machine when it comes to bit performance. A non rigid machine is the enemy of all bits, especially small ones.

IMHO people are gun shy about running bits. Probably caused by buying expensive ones, LOL. Here is a link to my machine roughing at 350 IPM, IIRC. That project was about 2 X 3 feet X 3 inches thick. The endmill was a cheap chinese 10mm cutting 5mm deep with a 70% stepover. Late in the video is some footage of a .25 ball nose finishing. It is sticking out of the collet about 3 inches. https://www.youtube.com/watch?v=tFA_1PJS32U Oh yea, the running time for roughing and finishing came in at about 5 hours IIRC.

Here is something to think about: No one wants to break an expensive end mill, that is a given. So buy a few cheap chinese ones and see what your machine can do, if you break them, oh well, it was only a couple of bucks. But what you might discover is that you can run your machine a lot faster. In my case, I have yet to break one. . . . .even at 800 IPM. Here is that video: https://www.youtube.com/watch?v=Pt8n43_YRjI&t=149s
"If you see a good fight, get in it." Dr. Vernon Jones

User avatar
Xxray
Vectric Wizard
Posts: 2114
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: Need advise

Post by Xxray »

Yep , have had the discussion of cheap chinese vs USA made before. I have tried cheap ones, in my case it wasn't so much that they broke but the cut itself was inferior, very inferior. Another one wouldn't fit in the .25 collet, shank was just a hair too small, but was too big for the next smallest size - Was not machined properly. Don't need that aggravation, my main bit I have used 100's of times in hardwoods, plexiglas, corian and more and is still going ,,, So I have found what I need and have no need to experiment, but I do have a few in reserve, some I don't even remember where I purchased them from.
Made in USA is a factor for me as well, I try to avoid chinese whenever I can as a matter of principle, and also generally try to avoid amazon as well - Even when it means spending a few more $$. I do think it would be rare to break any TBN bit unless you were really really pushing it or the bit was total junk, their geometry vs other bits like endmills is designed to be robust, and finish passes are usually not very demanding vs roughing or cutout.
Doug

User avatar
TReischl
Vectric Wizard
Posts: 3362
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: Need advise

Post by TReischl »

I hear ya Doug. For a while on FleaBay there were some characters who were peddling 6mm bits as .25 bits. The biggest problem I have with the 6mm bits is that sometimes they are a bit of a tight fit in a 6mm collet. Mostly this is from gunk that was not removed and appears to have hardened.

My guess about getting inferior cuts is because you probably use mostly carbide tooling. Cheap carbide is not going to cut as well as premium carbide. In my case I use all HSS tooling because it is sharper than even premium carbide and works better in the softer woods I usually cut. It also works better in aluminum for me. Watched a video the other day of a guy showing various carbide tools under a microscope, virtually all of them from cheap chinese to premium had a cutting edge radius. The chinese ones were the worst, not only did they have larger radii (due to the coarser grain of the carbide) but they also had chips and stress cracks on the cutting edge. I bought a cheap microscope a while back so I did the same thing. And yup, there are issues with cheap carbide tools.

Here is another interesting thing I discovered. Collets. The style we use on a router like a Porter Cable do not have the range of the ER style collets. If my PC router would be gracious enough to die one of these days I would love to get a real spindle on the machine. Not just for the collet but also the speed range. Over on the milling machine my top speed is 2500 RPM. Once in a while I will do some wood on it. I can easily do a 3/4 inch deep cut with a .25 endmill at a decent feedrate (no idea what that really is since my hand is turning the crank). Get good chips, nice cut, etc. It has a DC brushless motor with unreal torque at low speeds. Think of a 2.5 inch diameter forstner bit going about 75 rpm and not stalling in hardwood.
"If you see a good fight, get in it." Dr. Vernon Jones

User avatar
Xxray
Vectric Wizard
Posts: 2114
Joined: Thu Feb 17, 2011 8:47 am
Model of CNC Machine: CAMaster Stinger 1
Location: MI USA

Re: Need advise

Post by Xxray »

I have bben using ER's for quite some time. Funny you should wish death on your portercable, mine just bit the dust after almost a decade in service, rotating spindle seems to have locked up after months of showing signs of distress. May be able to repair it I don't know, if not I'll replace with another pc, a decade or service is impressive to me.
Attachments
IMG_4831.jpg
Doug

Post Reply