Fixing the jagged again(or text cleanup)

I was on the 3D SIGN FORUM this morning and was following a thread regarding cleaning up the jagged edges that can occur on vertical walls of a 3d relief. This process will work for all pixel based cad/cam software. This is something that comes up in numerous forum posts, etc. I did a tutorial a while ago, but it might not have been as in-depth as it needed to be!

First thing to be aware of is the difference between vectors and pixels. Pixels are the little cubes that are assigned various colours, or shades of grey that when combined side by side, make up any digital image. Pixels are easy to see if you zoom way-way in on a picture on the computer. Resolution defines how many pixels occupy a given space, usually Pixels Per Inch or PPI.

Vectors are precise mathematical lines and curves, that have no loss of quality when an image is scaled up or down.

So let's get down to business!!!!
This whole process only works if you keep your Aspire components separate. There's really no need for us to bake the text into the model. In fact I live by the the motto "I only bake when I have to" This motto applies at home as well ;)

I started my model at 24"X24" in Aspire, with the resolution set to standard (the lowest available option) It's always advisable to have the job size set to the smallest size that will fit the project. A 2" X 2" model will be very, very rough if the job dimension is 4' X8' with a standard resolution setting. This is because the pixels will be very large, compared to a job size of 2" X 2", where the pixels will be a whole lot smaller.

In the above photo, you can see the damage of a large workspace and low resolution with small text.

Here's a tighter shot of the resolution issue. Pretty apparent I'd say. This will definitely look poopy when it's machined!

 Heres the result of machining the whole 24" X 24" model. This was done with a 1/4" cutter with a 9% stepover. Looks perfectly acceptable on the log model....................

But not on the text close-up. You couldn't pay me to sand and file that clean, no way sister!
I'm gonna let Aspire, clean this up for me, and on our Techno cnc, it will be 100 times faster than by hand, and WAY more accurate! Re-toolpathing this whole model with an 1/8" cutter is unreasonable as well, as most of the model is perfectly fine

In the above image, the circle represents our .250" cutter. I've placed it right up against the original text vectors that were used to create the 3D text portion of our model.

An important point to remember is that in Aspire, a 3D toolpath is calculated to the CENTRE of the cutter. If I had used the original text vectors as a machining border, the cutter would have stopped at the point it is in the above image, the centre of the cutter right on the vector.
So knowing that the calculations are done to the centre of the cutter, we can plan accordingly!

So in the image above, the dashed line represents the centre of the cutter. This is kind of important to illustrate, because as the cutter will climb up and over the vertical wall to machine the text portion, it's going to leave a radius due to the ballnose cutter having a rounded tip.

We are going to machine of the radius around the text that was left by the .250" ballnose cutter. This will leave us a clean transitition between the woodgrain and the text. I'm going to some extremes in this tutorial, and going to jump right to a .0625" ballnose cutter for the cleanup. That is represented by the smaller circle.

I have dragged my .0625" circle inside the original vector. This looks like a good location to clean off those giant jagged edges as the cutter makes it's way around the text. We now just need to define that location in Aspire. As I said before, 3D toolpaths are calculated to the CENTRE of the cutter.

In this particular case it was around .008". So I simply selected my original vectors used to create the text, and offset them outwards by .008". This will allow the cutter to clean off the jagged edges without making the text to skinny.

I usually group both the vectors that I just offset. This keeps them all easily selectable.

With those vectors selected, I can now set up for machining.
This is where keeping the text component separate is important. We are going to hide the text component in the component tree. With this component hidden, Aspire doesn't "see" it, and therefore ignores it. If we don't hide it, Aspire will machine all those jagged edges again, making the text still look bad, and that's what were fixing. But as the woodgrain is still visible, it will protect that portion of our model. And as we have already run the .250" cutter, the text now exists physically on our model.

I chose the .0625" ballnose and assigned an OFFSET toolpath strategy. I am using an offset strategy as it will drive the cutter around the vectors smoothly, following each shape precicely, as opposed to rastering back and forth.

 TAA DAA! This is text I can live with. It will require NO additional cleanup by hand, and looks fabulous!

This seems like a long process, but it isn't in reality. You just basically offset your original vectors approx half of each cutter your using, hide the component your cleaning up, and assign an offset strategy. DONE!

This process lets you model at lower resolutions (which can speed up operations on slower pc's) And gives you great results.
8)
JO

Routering Aluminum by a guest!

<link rel="canonical" href="http://blog.cnccookbook.com/2012/03/27/10-tips-for-cnc-router-aluminum-cutting-success/" />
 
We have taken the last little bit off from some of the work at the shop. I say off, but the computer stuff is keeping me quite busy. We have been doing a lot of design work for some sets, as well as prototype modelling for some of our customers. As well as that, I have been doing some much needed work on our house. We put new windows in one side of the house in the late fall, and needed to finish some of the work related to that. Plus, with the weather being so nice, it was hard to leave the lake for the shop!

While doing some internet research, I came across a blogpost from "cnccookbook.com" It's quite an in-depth look at cnc routering aluminum. We do some aluminum machining on our Techno cnc, but not enough to have it down as an exact science yet!

This is a guest post by Bob Warfield, founder of CNCCookbook and creator of the excellent G-Wizard software. This post originally appeared on the CNCCookbook Blog.  I wanted to pass it along to our reader's as well with Bob's blessing at it contains a lot of useful information.  It’s a very clear explanation of how to successfully cut aluminum on CNC Routers. Very useful knowledge to have!

10 Tips for CNC Router Aluminum Cutting Success

Mar 27, 2012   //   by Bob Warfield   //   Beginner, Blog, Techniques  //  7 Comments

Folks often ask whether a CNC Router can cut aluminum.  They’re used to seeing the primarily cut wood and plastics.  My answer to this question is always, “Yes, if you do it right.”
There are a couple of things to remember about how aluminum (and other metals) are different from wood or plastics.  First, they have a much smaller “sweet spot” for optimal feeds and speeds.  If you leave the sweet spot, cutters start breaking, wearing out a lot faster, and surface finish is poor at best.  In fact, there are several sweet spots depending on what you want to accomplish:

 Metals have much smaller sweet spots (narrower range of acceptible feeds and speeds) than wood or plastics…

The second thing is that for aluminum (and some other metals), there is a “stickiness” factor.  Aluminum wants to stick to the tool.  In fact, it will do so to the point that it welds itself to the tool.  Once you have gummy aluminum deposits on your cutting edges, that tool is not long for this world, especially not at 20,000 rpm or more.

Despite these challenges, you can cut aluminum very successfully on almost any router.  Here are 10 tips for CNC Router Aluminum Cutting Success:

1.  Don’t be in a hurry

A CNC Router can cut aluminum, but it isn’t the ideal tool for it.  The price you’ll pay for success is slowing things down.  Note that I don’t mean to literally slow down your feeds and speeds, but your overall Material Removal Rates will be less than what can be achieved with a purpose-built CNC mill.  So relax and let the machine do its thing.  At the very least, a good sized CNC Router can fit a lot more material on its table than most any CNC mill.  Load it up, press the green button, and walk away.

2.   Use a Feeds and Speeds Calculator

Look, you’re going to approaching the limits of what your machine can do in all likelihood.  Cutting aluminum on a CNC Router is not a cakewalk, so let’s do it right.  None of this “cutting by ear” the old timers so love to talk about.  The ear can’t keep up fast enough as your machine skates around corners and through pockets.  One minute things are fine, the next you’re dodging the tip of the cutter that got broken off and flung across the shop.  All CNC’ers can benefit from a Feeds and Speeds Calculator, but when you’re near the edge of the performance envelope, you want to be particularly careful.  Of course we recommend our own G-Wizard Feeds and Speeds Calculator, but there are certainly others out there as well.  Use one!

Once you’ve got one, your first problem will be dealing with the recommended rpms being too low.  One of the issues for most CNC Routers is the spindle goes fast compared to a lot of CNC mills.  Your average new CNC mill maxes out at 10,000 rpm and many CNC Routers can’t go that slow.  Life for them begins at circa 20,000 rpm.  The next couple of tips focus on solutions for this problem.

3.  Use carbide coated cutters
One way to bump up the recommended rpm is to be sure you’re using cutters that are happy going that fast.  The measurement that determines this is called Surface Speed (for more on this and many other feeds and speeds hints and tips, check out our Feeds and Speeds Cookbook).  Carbide cutters can go much faster than HSS cutters.  Forget HSS and Cobalt for the most part.  A coating, such as TiAlN allows the cutter to go even faster.  Shop for carbide TiAlN coated cutters.  They cost a little more, but they may change your results so much it’s darned well worth it.
For example, say I need to cut a slot using a 1/4″ endmill. If I select an HSS Endmill, G-Wizard tells me it wants to run 5877 rpm and my 20,000 rpm router spindle won’t go that slow.  So I switch to a TiAlN Carbide Endmill.  Now the recommendation is 16897 rpm–we’re much closer.  This is with a Surface Speed of 1106 SFM.  You may be able to find a more aggressive SFM recommendation for your manufacturer’s tooling.  With aluminum, I’d go ahead and try 20,000 rpm for this cut.  It’ll probably be just fine.
4.  Use smaller diameter cutters
The other way to bump up the rpms is to use smaller diameter cutters.  Forget about 1/2″ endmills.  Drop down to 1/4″ maximum and typically less.  Because you’re going to smaller diameters, you want more rigid cutters lest tool deflection starts to be a problem.  Carbide is much more rigid than HSS, so this is one more reason to favor carbide.
Looking at our example in #3 of the carbide cutters, suppose that instead of a 1/4″ endmill, we are using a 3/16″.  That seemingly small change has now kicked up the recommended rpm to 21241–very close to our 20000 rpm spindle.  It’s easy for us to slow that down to 20K rpm and pick up a little extra tool life.
The moral of the story is to carefully match your tooling to the capabilities of your machine.

5.  Be paranoid about clearing chips

Recutting chips breaks more cutters than most any other thing I see happening.  Be paranoid about clearing the chips.  Don’t count on a nearby vacuum dust collection system unless you have personally verified it sucks the chips out of even the deepest cuts.  More reliable is an air blast fixed to the spindle and pointing right at where the cutter meets the material being cut.  If you’re standing there, nozzle in hand (or worse a brush) thinking you can keep things clear, you’re not paranoid enough about clearing chips.

6.  Watch cut depths and slotting–they make it harder to clear chips

The deeper you cut and the closer to a slot the cutter travels in, the harder it is to clear the chips out of the bottom of the hole.  Make more passes to cut down to required depth and to open up the shallower depths for better access.

7.  Lubricate with a Mist

Assuming you’re suitably paranoid about those chips, the next issue is providing lubrication to cut down on the tendency for the chips to stick to the cutting edges.  You pretty much have to use some kind of lubricant.  Since you’ve presumably already rigged up a compressed air blast, you may as well run coolant mist through the same mechanism.  In fact, buy a mister to provide air blast and coolant mist.  It’s easy and inexpensive.

8.  Don’t slow down the feedrate too much!

If you go too slow on your feedrate, you run the risk of making your tool rub rather than cutting.  This is a much bigger risk for CNC Router users than mill users simply because the spindle is going so fast.  In order to maintain recommended chiploads with rpms that high you’ll have to keep the cutting moving smartly.  Our 3/16″ cutter at 21K rpm wants to feed at 91 IPM, for example.  If you slow down too much, say to 1/4 of that, many will think they’re babying the machine and tool.  Nothing could be further from the truth.  If you wind up going slow enough that the cutter starts rubbing at 20K rpm, you’re going to heat up the whole works and drastically shorten your tool life.  For more on this rubbing phenomenon, see our article on chiploads and surface speeds.

9.  If your machine can’t feed fast enough, use fewer flutes and increase cut width

Normally, we use 3 or fewer flutes with aluminum anyway–don’t try a four or more flute cutter in aluminum!  The reason is that aluminum produces especially large chips.  The fewer the flutes, the more space between the cutting edges, and the more room for the big chips to escape and be blown away.  With too many flutes, the chips back in too tightly,  jam up the flutes, and pretty soon you have a broken cutter.  Let’s suppose you are using your feeds and speeds calculator, and you come up with a situation where your machine just can’t move the cutter fast enough.  For example, taking our 3/16″ example at 21K rpm, let’s say we’re cutting an 0.040″ wide cut.  G-Wizard suggests feeding a 3 flute endmill at 166 inches per minute, but your CNC Router can only cut accurately and reliably at 100 IPM.  What to do?

The answer is to try fewer flutes.  A 2 flute cutter only needs a feedrate of 110 IPM.  Slowing that down to 100 IPM is not going to run a rubbing risk–it’s only 10% slower.

BTW, we’ve been talking about cutting aluminum, but you can hit this problem even worse with wood because you can cut the softer material so much faster.  Plug in these values and select Hardwood in G-Wizard and it wants to go 883 IPM at 20,000 rpm!

Here’s a tip: they even make 1 flute cutters for precisely this reason.

If we take the scenario down to a single flute at 20000 rpm GW now recommends 294 IPM. If you’re burning the wood, it’s probably because you’re feeding too slowly and the cutter is rubbing.  BTW, I love watching a fast moving industrial CNC Router blasting through wood and shooting up a blizzard of chips and dust.  Cool beans!

The other thing to be aware of is what’s called “Radial Chip Thinning“.  If your cut width is less than 1/2 the cutter diameter, you need to speed up your feedrate because your machine is producing unnaturally thin chips due to Radial Chip Thinning.  Here again, you think that by taking super thin cuts and slowing the feedrate down drastically.  Instead, because of radial chip thinning and rubbing, you’re drastically reducing your cutter life.  The G-Wizard Feeds and Speeds Calculator automatically factors in radial chip thinning to its calculations.

10.  Use a Horsepower limit to derate for rigidity

Okay, you’ve mastered the other 9 tips, and thinks are going well, but you’re now running up against the rigidity limits of your machine.  If you plow in with full power, bad things happen.  The machine chatters and destroys the cutter, surface finish is lousy, or the machine deflects and cuts very inaccurately.

Cutting forces for metal are likely to be much higher than for wood and CNC Routers (sometimes called Gantry Mills) are considerably less rigid than equivalent CNC Mills.  This is just a fact of life.  If nothing else, compare the work envelope of the mill (much lower than a router) and it’s weight (much higher than a router) against a CNC Router.  Except for the biggest industrial Gantry Mills, there is no comparison.  And because of that, no way that machine is as rigid as a CNC Mill.  So, we have to compensate.

We don’t know the exact rigidity of a given machine.  There’s not a published spec we can use to compare or calculate from.  But, we can use spindle power as a proxy.  It is that power “pushing” against the workpiece while cutting, that the rigidity must fight.  G-Wizard has the ability to calculate a “de-rated” spindle power that matches the work envelope and weight of your machine to a spindle power that is appropriate for that level of rigidity.  The results may surprise you, but they’re based on real empirical measurements.

For example, suppose you have a 4′ x 8′ router with 20″ of Z travel that weighs 1000 lbs.  Note that even a fairly lightweight commercial CNC mill, like a Haas TM-1, will have travels of 30″ x 12″ x 16″ and a total weight of 3240 lbs–a much smaller envelope and a lot more weight.  To perform at this kind of level of rigidity (and a TM-1 is not exactly the pinnacle of rigidity either) requires derating horsepower to 0.17 HP.

Derating will take our numbers way down–22K rpm and 79 IPM for the full slot with a 3/16″ inch and a 2 flute.  But, we’ll get the job done with better surface finish, accuracy, and less tendency to deflect the machine frame or chatter.

Conclusion

Machining aluminum with a CNC Router is absolutely doable with most any router.  It’s just a matter of matching your machine’s capabilities to the “sweet spot” feeds and speeds requirements of the material through wise selection of tooling and cutting parameters.  Add to that the need for lubrication and being paranoid about chips piling up and you’re ready to tackle an aluminum project.

 --------------------------------------------------------------------------------------------

I hope you guys stop and visit the  http://blog.cnccookbook.com blog as it's definitely worth bookmarking!!!
8)
JO

Clamydia Finally!

 I found the final print spot for our Chlamydia necklace build on the Westside Studio blog!

 The final looks great! Plus it's kinda fun to creep the Westside blog!!!

Here's the build progress if you didn't get a chance to see it before:


Saturday I went into the shop to machine the Chlamydia necklace. I should note that this necklace is for a print campaign bringing awareness to STD's. The art department supplied the vector format for us. I had to adjust the size a little to accommodate the size of the diamonds we were using. These are cubic zirconia flat-back diamonds, not real ones. Otherwise I would have just left the country with them and saved all the work!
I brought the file into Corel Draw first, as I needed to figure out where all the stones were going to go (there are actually over 200 of them). I could have done this in Aspire, but somethings are better in Corel for me.

When I was happy with the way all the stones fit, I exported the file out for use in Aspire. I didn't need the stone layout for machining, so I just deleted them. I decided to mill this from 1/4" T6061 aluminum so I could polish it to a high shine. Paint just wouldn't cut it for this job as it's a fairly tight shot.

I toolpathed the center using a 4 flute 1/8" endmill. I probably could have been more aggressive with my step down passes, but chose to take it lightly. The outside profile machining was done with a 1/16" endmill so I could get into most of the kerning. After it came off the machine, I started the painful part of filing the edges with a very fine file to remove all the machining marks. After the edges were flat, I moved to the buffing wheel. The polishing took quite awhile, using the dremmel to get into the tight places was nearly impossible, but perseverance paid off in the end.
Today was set aside for laying the stones in. I filled the pocket text with Sherwin Williams automotive clear coat. This has such a high gloss to it. And because it's a urethane product, it's also a serious glue. The working time with it would be around 4 hours, so I could brush it in each letter at a time, then using my labelled stone placement chart I made earlier, I placed the stones in their location. The clear will harden overnight, locking the stones down.

It took a very long time to place the stones. I had used tweezers for this task, but some stone would drop and roll away. Some would land upside down in the urethane, which means I would have to turf them, because if the clearcoat gets on the faceted surface, they lose their sparkly bling.

By the end of the day the stones were all placed. Tomorrow we are delivering it to the studio. First thing in the A.M. I will mount the rings that the chain connects to, and hook up the chain.
This was a really great job to get! I can't believe I get to do this stuff sometimes.
8)
JO