Blog Archives

Index

Current

The CNC Cookbook Blog

Check out the G-Wizard Machinist's Calculator...

8/28/10

Climb Milling a Must for Thin-Walled Parts

Thin walled parts are a real pain because the thin walls want to vibrate like a tuning fork. When that happens, you've got trouble, big trouble, and its name is chatter. I was reading a fascinating article recently that made the point that when milling thin walls, climb milling is a must. Because climb milling cuts with the part instead of against the part, it transfers less energy to the part and is therefore less likely to make that thin wall vibrate.

Using cutters with more flutes is also helpful. Depending on the engagement angle of the cutter, the more flutes, the more that are engaged on the part, which helps stabilize it. With a 2 flute cutter, there is only ever one flute engaged, which is the worst case of beating the material until it vibrates. Higher helix tools help too, because they pull up on the part, which keeps it in tension and reduces its tendency to chatter.

If you're working on a material that doesn't dissipate heat well, like titanium, thin walls are a problem because the heat builds up more. You'll need to focus on better cooling, and either lower the spindle speed or reduce the cutter engagement to keep the heat down.

If you reach very far down into your thin wall cavity, you'll need to look at tapered shanks or even tapered tools. Even though you're only cutting at the tip, having that thin wall rubbing on the spinning shank still injects vibration and chatter into the job.

Tool deflection is a big deal with thin walled jobs. Be sure to keep it to a minimum. G-Wizard's Cut Optimizer will tell you how much you can cut for a given tool deflection allowance.

Here is another tip: make sure your tool's radius is less than the minimum internal radius needed for the part. This insures the tool is always moving. If the tool radius is the same, it will come to a stop in the radius of the part and that starts the chattering again. Keeping the tool radius a little smaller than the minimum part radius is a good idea in general, not just for thin walled parts. It will lead to a better surface finish.

A challenge is designers who are unaware of the relationship between cutter radius and the radii in their designs. They make the radii of their parts in round numbers because that's the typical way people think. So, for example, the smallest radius may be 1/4". But cutters are sold in round number sizes too, so you've probably got a 1/4" cutter on hand and your next size down may be 3/16". There are two good possibilities to make life easier:

- Get your designers to make their internal radii just slightly larger than your standard cutter sizes. That's the best answer if it doesn't matter to the design, and its very easy to do.

- Lay in some cutters as close to the standard sizes as possible but just smaller. For example, MariTool lists a 15/64" endmill right below the 1/4". It's more expensive, unfortunately, because they aren't called for as often. Or you could drop down further to 7/32" and save a little more money.

There is a trade-off in tool rigidity that creeps up pretty fast, so don't downsize the endmill too much. For example, G-Wizard's Rigidity Calculator tells us the following:

If a 1/4" endmill is a factor of 1 in rigidity, the 15/64 is only about 76% as rigid, and the 7/32" is 59% as rigid. If we fall all the way back to 3/16", our endmill is now only 32% as rigid, which is really going to slow down our production.

Now you know what those odd-sized endmills are good for!

8/22/10

Deciding on Best Depth and Width of Cut When Milling

I got a note recently from a G-Wizard user who wanted to know how to decide on best depth and width of cut when milling. It's a great question. Most machinists, I suspect, use rules of thumb and habit more than anything else unless the situation dictates something in particular based on the dimensions of the feature being machined. They're used to using some fraction of the cutter's diameter or some figure that they got to some other way through habit (40 thousandths or some such is what they've always used). Perhaps their CAM program has a hardwired default that is a percentage of the cutter's diameter.

But these values, while they have worked over time, are not necessarily optimal figures with respect to material removal rates, tool deflection allowances, or a host of other variables we might choose to consider. What's a more systematic way to approach the problem?

First thing is we have two variables (width and depth of cut), so it's hard to make progress unless we can nail one of the two variables down and focus on the relationship of the other. It's usually pretty easy to nail down one of the variables based on the situation. Let's divide our work into two categories:

- Slotting: I'll generalize this to be any situation where the material to be removed is very close to the cutter's diameter. It may be a slot, or it may involve interpolating a hole or pocket that's only a little bit larger than the endmill's diameter.

- Pocketing: Here again, I will generalize this to be any situation where the cutter's diameter is quite a bit smaller than the dimensions of the material to be removed. That doesn't mean there isn't some inside radius or other feature that isn't more like the slotting example, but for the most part, we have some room to work in. Note that profiling will be considered to be the same as pocketing for this discussion.

Okay, so now we have to take the task before us and decide whether it is closer to slotting or pocketing. The reason I've defined these two the way I have is that it informs our choice of which variable to work on first. If we are slotting, the cutting width is the first variable. If we are pocketing, the cutting depth is the first variable. Why?

When slotting, the feature is very close to the cutter's diameter in size. We can't take a 1/2" endmill and use it to make a 1/4" slot. In general, we want to use the largest diameter endmill that fits the feature, and then we pretty much have to make at least one cut that is full width. Once we're cleared that cut, anything remaining is handled the way we would under pocketing. So, when slotting, we focus first on cut width and make that the cutter's width to get started.

When pocketing, our limitation will be the smallest inside radius we have to deal with as well as the depth of the pocket. Remember, it may be advantageous to make two passes. The first with a cutter that has a diameter too large for the smallest inside radii we have to deal with. That's a roughing pass that uses a larger cutter just to get done faster. The second pass is a finishing pass, and must use a cutter whose diameter is less than or equal to that required to reach into the smallest internal radius the pocket holds. Note that we can go around an outside radius (a boss) with any diameter cutter, it is the inside radius that limits us.

So, we pick a cutter that is either as big as the smallest radius, or we choose to go two passes and go with a larger cutter. Let's leave the two pass issue aside for the moment, because figuring out when that is optimal can take a bit of trial and error. Its similar to think of one pass. Given that the cutter is chosen, we can choose just about any width of cut we want. So how do we nail down a variable when pocketing? On the slotting case, I like to nail down cut width. On the pocketing case, I prefer to nail down cut depth.

In general, we get a nicer finish if we cut the pocket in as few layers as possible. CAM programs are good at layering down into the pocket, so we can pick arbitrary depths of cut. If I can, I like to do it in one layer for a pocket that isn't two deep. If not, I prefer the depths of the layers to be equal. In other words, I wouldn't go down 1/4", 1/4", and then 0.19" on the third layer. So pick a layer depth that satisfies that criterion.

Now, in both cases we have locked one of the two variables--slotting locks width, pocketing locks depth. We need to determine the best value for the variable we left floating based on the value of the one we locked. This is where the G-Wizard Cut Optimizer makes it easy. Enter the values you know for the cut and let the Optimizer figure the value for the floating variable.

For example, let's suppose we need to cut a pocket that is 3/4" deep in 6061 aluminum. The smallest internal radius is 1/4", so we've decided to use a 1/4" 3 flute carbide endmill. Here is the problem set up in G-Wizard:

Material, Tool, Tool Diameter, Flutes, and 3/4" Cut Depth Entered...

Now we can invoke the Cut Optimizer just by pressing the "Rough" button:

As you can see from the red arrows I added, for a 3/4" depth of cut, this endmill can handle no more than 0.1799" width of cut when roughing. Let's round that down and go with 0.170"

Press the finish button to see what sort of finish allowance we should have the CAM leave for our finish path and we get 0.0052". That's a pretty light pass, but 3/4" is deep for this 1/4" endmill. Here's an interesting thought: if we reduce tool holder to tip length to 0.9" instead of 1", we can increase that cut to 0.0095". That gives you an idea of how important it is to keep the tool stick out as little as possible. I'd be inclined to go with choking up on the tool and a finish width of cut of 0.009" were this my job. The other thing to consider is two levels of finish pass. If we don't mind taking two levels and still choke up on the tool, we can get 0.015" width of cut for the finish. That's about as much as I like to take on a finish pass.

The problem with this cut is its a little bit deep for our 1/4" endmill. That's a 3:1 ratio of diameter to depth. We can tell its straining because the max recommended widths of cut are so light. If I had a CAM program that made it easy to make the roughing pass with a bigger cutter, I would be tempted to jump in with a 1/2" endmill (or maybe even larger) for the roughing pass and then go to the 1/4" for finishing, but you get the idea.

The slotting case is pretty similar, except for that case, instead of trying to compute the width of cut, we want to use the optimizer to figure out the depth. For example, if we continue with our 1/4" 3 flute, let's say we need to cut a slot 0.300" wide to a depth of 3/4". Our plan is to cut a full slot 0.250" wide down the middle, and then finish it up by cutting the remainder on each side. How deep can we make our full slot passes? Once again, dial up the initial parameters, and this time, hit the "Slot" button. For roughing, the Cut Optimizer tells us we can cut to a depth of 0.3466" before we get too much deflection. Two passes at that depth will get us to 0.6932" deep. That leaves 0.0568" on the bottom for us to finish and 0.0259" on either side for the finish pass. Remember, we're not cutting a full slot for the finish pass, so we treat it just like we did our pocket to figure out the width and depth of cut.

That's all there is to it. To summarize:

1. Decide whether you are slotting or pocketing.

2. When slotting, pick a value for width, and use Cut Optimizer to decide depth.

3. When pocketing, pick a value for depth, and use Cut Optimizer to decide the width.

If you approach the problem this way, you'll maximize your MRR's while minimizing your tool deflection as appropriate for either roughing or finishing. That's a much more optimal approach than the old wet finger in the wind!

For more thoughts on cutting parameters when milling, check out the Milling Surface Finish page.

8/18/10

Cutting Chatter When Precision Boring

I just came across what looks like a great blog from Criterion, the boring head people. They had a great tip to reduce chatter: make sure your depth of cut is greater than the radius on your cutter. It makes sense, and should apply when turning too. Here is how they explain it.

Consider the cutting forces when the insert is cutting less than the radius:

See how the forces (arrows) are largely trying to push the insert out of the cut?

With a deeper cut, there are more arrows acting to stabilize the forces so they're not all trying to get the insert to deflect and skip over the cut.

The result is a better finish and less likelihood of chatter. Having to increase depth of cut in this situation is just one of the many counter-intuitive situations we encounter when machining!

8/18/10

The Web is All About Sharing

The Web is a Social Place. It's all about Sharing your finds with others. While search engines like Google are great, and I use them constantly, often the real gems come via friends who tell me what they've found and liked. For a long time I've kept a CNCCookbook page on Delicious of all the many interesting pages I come across. They have a tool bar for your web browser to make it easy to bookmark interesting things you come across. Check it out (click on that link above) to see nearly 2000 articles with my summary of what interested me as well as tags like "mill", "lathe", "cnc", "tooling", and "workholding" to help you focus in on topics.

That database of Delicious (love the name) links is my "newswire" for writing posts here. I grind through a lot of information so consider it sort of a Reader's Digest. If you like CNCCookbook, you'll probably like a lot of those articles too.

Meanwhile, you may have noticed all the CNCCookbook pages now have their own sharing bar up in the top left corner near our logo. It looks like this:

Go ahead and check it out with your mouse, either the one right above or top left. It will show you a list of all the popular web services from email to Facebook to Twitter to Delicious where you can share whatever CNCCookbook page you're on. Please help us to get the word out about CNCCookbook and G-Wizard by sharing. You'll be doing us a favor, and you'll be doing all of your friends who like to see what you like on the web a favor too!

If you can, take a minute now to share with the new button, or just send an email to 3 of your machinist friends or coworkers to let them know about us.

Thanks, I really appreciate it!

8/17/10

Of Pallets and Parts

I've always like the idea of pallets that can be set up with new parts while the CNC machine is working on another set of parts. Sort of like quick-change fixtures of a sort. You know it has to contribute to productivity, because when the machine stops you can swap the pallets real fast and the spindle turning again while you pull the parts of the finished pallet and set new workpieces in place to go back in. But how much productivity improvement is possible?

I was reading through a post on the LinkedIn CNC Machining and Manufacturing Network (pretty good group, actually) and saw some interesting figures being quoted by a former sales guy from System 3R. I look their web site and think large scale manufacturing and keep moving (I'm more interested in small operations and techniques that work for a lot of different parts), but what René van der Peet had to say was exactly on target for smaller shops:

- A machine, without any equipment, used during daytime in one shift, produces an average of 800 billable hours each year.

- A machine with just a manual pallet system, used during daytime in one shift, produces an average of 1600 billable hours each year.

- A machine with automated pallets, used during daytime in one shift, produces an average of 3000 billable hours each year.

Those are amazing productivity increases. Heck just the manual pallet system seems like it would pay for itself very quickly. This experience was gained with European machine shops in the Benelux area.

Small shops (and Big ones too, but the small mom and pop shops may be adding their first operators, so it is a bigger decision) often have to consider whether it makes more sense to hire employees are invest in better technology (e.g. faster CNC machines or tooling). Doubling, tripling, and quadrupling the throughput of your machines without adding more employees seems like its worth looking in to if you have enough work to absorb the capacity.

Failing the work, it may free enough of your time to let you spend time doing non-billable things like designing and prototyping your own products to sell.

The downside is it will require the up front investment, as well as reworking your fixtures and processes to work with the pallet system you choose.

Someone else on the thread mentions that System 3R is super accurate with respect to repeatability because its made for EDM work! Clearly that's very cool for certain kinds of jobs, but it may be that a less expensive investment is also workable. I'll have more to say about such fixturing over time as its an area I'm very interested in.

Drop me a note if you have experiences along these lines!

Ballnose Surface Finishes

It's a small world, I guess. No sooner did I get done adding a section to my Turner's Cube page showcasing Widgitmaster's lathe-turned versions when I find him asking a question on CNCZone about how to calculate stepover to achieve a desired finish when profiling with a ballnosed cutter. As it happens, this function is built into G-Wizard like so:

Ballnose information appears below the RPM and Feedrate when the "Ballnose Cutter" choice is checked. It provides the effective diameter based on depth of cut and for a given scallop height will tell you the RA/RMS Surface Finish and required stepover. In this case, to achieve a maximum scallop height of a tenth (0.0001") for an RA finish of 100, we need a 0.011" stepover. That's about 2.2% of the tool's diameter.

Feeds and speeds for ballnosed cutters can be a bit tricky because the effective diameter of the tool is based on the cutting depth whenever you're less than have the diameter of the tool deep. Think about it, the end of the cutter is a ball rather than the usual cylinder shape. You have to calculate the effective diameter based on how far the ball is into the workpiece.

8/15/10

Interpolating Holes vs Twist Drills

They say nothing removes material faster than a twist drill. Just one problem, it only removes a cylinder of it, so it can't really profile or pocket (the exception being pluge roughing, but I'll save that for another time). Although, profiles and pockets often begin with the need to get the endmill down to proper cutting depth. Given that you know how long a tool change takes on your CNC mill, how many such plunges do you think are required before you'd be better off to use a twist mill to do the initial plunge and then let the endmill interpolate off of that?

It turns out to require fewer holes than I would have thought, and it's pretty easily to calculate with a little help from G-Wizard to get the feedrates.

For a 1/2" HSS 2 flute in 6061, GWiz gives a plunge feedrate of 4.96 IPM. A 1/2" HSS Twist Drill can be fed at 15.28 IPM. That difference in speed, with the Twist Drill being a lot faster, has to make up for the toolchange time. In fact, let's say we want to change twice--from endmill to twist drill and back. Further, lets say our toolchange time is 5 seconds.

Based on all that, if we use the twist drill to drill just 2 holes we are 6 seconds ahead. If we have multiple parts laid out on the table, its pretty easy to see how this multiplies in a hurry to our advantage.

Of course we'd need a CAM program that's capable of drilling all the holes with the twist drill and then going back and pocketing off those holes without cutting too much air. I don't think my CAM program, OneCNC, is nearly smart enough to figure it out on its own. But perhaps I could convince it to do the right thing with some suitable fiddling. If nothing else you could create a CAD drawing that showed the holes drilled as solid features not to be milled into. It would make an initial helix pass down around the outside of that slug, and you could bump up the feedrate there to regain the lost speed. Make the slugs hole size minus the tool diameter in side, so ideally you want to use a twist drill a bit larger than your cutter diameter. Maybe 3/4" for my 1/2" endmill example.

Of course if you have a 1" indexable drill sitting in the changer, you can bump the feed up to 38 IPM and really make some holes! Incidentally, I have read accounts of folks leaving a 1" in the toolchanger on lathes just to make boring go faster on bores that are more than 1". Same idea.

The interesting thing is not only is the twist drill often faster, its a cheaper tool to put the wear and tear on. Click here to download the quick and dirty worksheet I used for my calculations.

There are tons of tradeoff decisions like this to be made when setting up a CNC job. For example, the usual inclination when profiling or pocketing is to select a cutter that is just equal to the minimum radius to be machined. But you're penalizing the whole cut with that smaller tool. Most of it could be handled by a bigger tool. Given a knowledge of which tools are in your changer, and the possibility of using 2 tools instead of one (rough with a larger radius, finish with a smaller), and a knowledge of your tool change speed, how much savings can you get using 2 tools instead of 1 and is it worth it?

Remember, the larger tool not only removes more material just by virtue of its size, it is also tremendously more rigid as G-Wizard's rigidity and cut optimizer modules will show you. What if the roughing pass with the larger tool can cut full depth while finish takes 2 steps to get to full depth? Now the 2 tool approach really has an advantage.

CAM programs have a facility called "Rest Machining" that seems the logical way to approach this sort of thing. Rest Machining keeps track of what a particular operation failed to machine so that subsequent operations know where the air is and can avoid cutting it.

I'm Back, Though Not 100%...

People were starting to write and complain they hadn't had their CNCCookbook "fix" in a while. Sorry about that folks--I was off in Cozumel, Mexico on a diving vacation. All work and no play makes Bob a very dull boy. At least now I'm back, though not 100%. I seem to have either a particularly bad cold or a mild case of the flu. It's definitely on the mend, so I wanted to get back to writing some Cookbook posts again.

Drawbots

I love the idea of Drawbots!

What's a Drawbot? It's a little CNC machine used for drawing or painting. They're typically 2D devices that are suspended on cables. If you've been to an amphitheater event any time recently that had a lot of video, you may have seen a video camera suspended on something similar. Here is a typical Drawbot:

In this case, the Drawbot hangs on the wall as a piece of kinetic art. It takes hours or days to finish a piece, but its always busy doing something, so is interesting to look at. Here's a close up of the piece its working on:

There's a fair amount of scoop on Drawbots over on the Makezine site. As I understand it, you can run a Drawbot with Mach3 by putting the correct math into the formulas for the axes. In this case, we have to simulate X and Y motions using the string droop.

I'll have to try and make one some time. I've seen some set up for doing large commercial sign painting that seemed cool. Van murals, anyone?

Ferrari V4 Motorcycle

Crazy cool is all I can say:

Nothing like a good rendering to stimulate the appetite, but it leaves you feeling hungry, doesn't it? How long before some intrepid CNC'er decides they can't wait to have one, I wonder?

Earlier Entries in the Blog...