Topic for Forum Member Rando

Discussion about the CNC Shark Pro Plus HD

Moderators: al wolford, sbk, Bob, Kayvon

sharkcutup
Posts: 408
Joined: Tue Mar 08, 2016 5:23 pm

Topic for Forum Member Rando

Post by sharkcutup »

Machining aluminum

5" x 5" Block by 1.0" thick Aluminum Material Stock

2.0" diameter x .5" high circle centered on block

I am using VCarve Pro 10.507

1) What program do you use for cutting aluminum parts?
2) If you use VCarve Pro or Aspire how are you programing something like this?

Reason for asking I have found that the pocketing toolpath only works from inside out on a Offset Climb or Conventional Cut Direction.
I am looking for something that works on 5 by 5 block taking little off at a time on each stepover starting from outside working in to 2" diameter circle.

I know you cut aluminum a lot so thought of you (sorry to say :roll: ) when problem arose with VCarve Direction (inside to outside versus outside to inside).

Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 11.554

User avatar
Kayvon
Posts: 552
Joined: Tue Oct 21, 2014 11:46 pm

Re: Topic for Forum Member Rando

Post by Kayvon »

sharkcutup wrote:
Tue Sep 29, 2020 12:00 pm
I know you cut aluminum a lot so thought of you (sorry to say :roll: )
You have an interesting way of asking for someone's help.

sharkcutup
Posts: 408
Joined: Tue Mar 08, 2016 5:23 pm

Re: Topic for Forum Member Rando

Post by sharkcutup »

YUP! He is a busy fellow. Do not really wish to disturb him, LOL!

Just curious as to what program he may be using and how he approaches that type of carving with VCarve because VCarve does not have the ability to change the direction of an pocketing toolpath from starting from the inside to the outside versus Outside to the Inside. (No way that I could find!!!)

Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 11.554

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Topic for Forum Member Rando

Post by Rando »

Give me a few....I'm using VCarve 8.5, but that's where I started, so it can be made to work.

Sorry, I'm currently hot-and-heavy applying toolpaths to an updated version of that gantry design for that one customer. Been at it for a week now...no, seriously...it's well over 300 individual toolpaths. Sure am glad momma told me to grow up and learn programming!

anyway, should have information for you by this evening.

What's the ability for spindle/router speed control? And, which one is it?

Cheers!
Last edited by Rando on Tue Sep 29, 2020 4:24 pm, edited 1 time in total.
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Topic for Forum Member Rando

Post by Rando »

one thing that's not entirely clear to me: Will the part end up having a round boss that sticks up 0.5"? Or will it be a square block with a circular hole 0.5" deep? Sorry for my confusion.
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Topic for Forum Member Rando

Post by Rando »

So, a couple things:

0) Before anything, ANYTHING, remember that the Sharks are really squishy. High cutting forces will pull that HDPE in ways that will make you cringe, and will break expensive bits. So yes, the cutting here will seem paltry and tiny compared to cutting soft wood. The alternative is broken bits, ruined collet inserts, and ruined parts.

1) Before I create the toolpath, I decide what the F&S should be. For a 0.25" 2FL carbide end mill with 0.020" corner radius*, cutting 0.050" deep, with 0.0125 (5%) stepover as a nominal starting point for this kind of thing, my F&S calculator--when set to calculate very light "10% finishing" cuts--says the following:

16500 RPM, 44 IPM horizontal, 9.6 IPPM Vertical. That will give you about 0.32 oz-inches of torque on a 3HP spindle. If it was a "weak" steel machine, it might produce a bit deflection on the order of 50 micro-inches. But, it's not, so expected ~ 0.010" deflection in the machine.

One thing to remember about aluminum: going slower is NOT your friend. If you cut the feed rate, you MUST cut the spindle speed as well, and you can only go so low before you're outside aluminum's viable SFM cutting range.

Now onto the Vectric portion.....

The "proper" style of machining these kind of pocket (assuming it's not a boss) on a machine like ours is called "high speed machining", HSM. In the case of this round pocket, the difference is clear. In the Vectric (8.5, I have to assume they have HSM by v10) toolpaths, each cut in the circle is two arcs, then a horizontal chomp to the next outward level, then two more arcs, and so on. In HSM, that horizontal chomp doesn't exist. Instead, the two arcs are mathematically blended together, and all you have are nearly-circular arcs. While not specifically "required", not having that horizontal chomp removes what are HUGE spikes in torque presented to the spindle. Those spikes are hell on the sharks, because they can turn a horizontally-moving bit into a an expensive broken drill-bit when that happens in aluminum. The metal can actually melt under the bit and then weld the bit in place. Not fun, and I have a JAR of these broken bits :(.

In addition, ramping and spiraling down into the material is required. Vectric 8.5 only does ramping, but it will go back-and-forth to get down to depth. Most ramping into aluminum is done in the 2.5° to 3.0° range. Don't plunge directly into aluminum on a shark; it won't go to the correct depth because of the cutting forces. Likely your version can do spiral/helical ramping by now.

Thus, the trick is to use very small stepover, and relatively high feed rates. (and you have to use different feed rates for different cuts...a slot is NOT like cutting a pocket).

The below attachment shows the parameters I chose. Note the thin depth of cut and the narrow stepover.
VectricRoundPocketInAluminum.GIF
More in the next messages....
Last edited by Rando on Tue Sep 29, 2020 5:37 pm, edited 3 times in total.
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Topic for Forum Member Rando

Post by Rando »

Now....what do **I** use? Not Vectric. At least not the v8.5 of VCarve Pro that I have. I use Vectric now only for engraving toolpaths.

For 3D solid modeling I use AutoDesk Fusion 360, though their upcoming license changes (starting October, 2020) are infuriating.

coming out of Fusion, I use STL files to go to 3D printing, and STEP files to get to machining.

Theoretically I could use the Fusion CAM stuff, but I already spend a chunk of change on....

BobCAD/CAM is what I use for toolpath generation. I have their "3-Axis Pro" package, which includes a whole slew of 2D and 3D toolpaths, with way more and better options than Vectric has. Except for tabs: both suck equally on tabs ;-).

I wrote custom post-processors for all the GCode-generating tools I use, so that they toolpath blocks can be detected in another program I wrote.

I've talked about that one before: GCodeSG, or GCode Splatter-Gather. It takes all-in-one GCode files, breaks out the individual toolpaths, and then re-joins them together based on the order specified in a simple text "join file." In Vectric, very often you get to load every single toolpath individually, and turn them individually. With mine, I can group them into paths that use the same setup and bit. On the current project, it lowers the total number of toolpaths I load from over 300 to under 50 for the ten machined parts.

And, of course, there's my PilotFish. That's an arduino based power controller. The BobCAD and Vectric post processors, based on UI-chosen options (by the user in BobCAD, by default in Vectric), inserts chunks of GCode that send 35ms pulses out the router power-on line. The PilotFish detects these, and interprets them to turn on, turn off, or pulse any of 10 channels. Each channel has a 10A form-C set of contacts, and an 0.3A form-A set. I built a bunch of remotely-enabled power control boxes, so the chip blower and other things don't draw power near the CNC. It's a fun trick, and makes it trivial to control the chip blower and lubricant mister. Each toolpath turns them on and off as needed for that toolpath, with no input from me beyond setting an option in BobCAD. It's slick.

BobCAD is cool, but BobCAD is spendy. Getting the full-meal-deal even for our 3-axis machines will run upwards of $4K at full price. I got them at their fiscal year end once when sales was desperate, and got a decent deal...which they then clawed back at the next version upgrade that happened in six months. Oh well, I rely on the tool and the quality of results pretty much every single day.

So....does that answer your question, sharkcutup?

Cheers to everyone!

Rando
Last edited by Rando on Tue Sep 29, 2020 5:31 pm, edited 2 times in total.
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Topic for Forum Member Rando

Post by Rando »

And, if you're thinking boss instead of pocket, simply use the stock-material bounding box in the pocketing vector selection, and you get this
VectricRoundPocketInAluminumBoss.GIF
I tend to oversize that box by 0.020" so it's sure to clear off all the top surface.

Cheers!

Rando
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Topic for Forum Member Rando

Post by Rando »

Oh....and when you can, always use CONVENTIONAL milling in aluminum. Not always, but pretty much near-enough. The thing is, the squishy shark lets the bit get pulled into the material on conventional cuts, and the chips have a tendency to weld themselves onto the surface, mucking with the finish. Not so with climb milling, because the chips are spit out behind the cut, and the tendency is to lift the bit away from the material, not into it. Add in radiused corners on the flute tips, and the diving isn't nearly as much a problem.

And, remember: bits go dull. Don't expect that carbide endmill, even a $100 one, to last forever.
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Rando
Posts: 757
Joined: Tue Jan 06, 2015 3:24 pm
Location: Boise, ID
Contact:

Re: Topic for Forum Member Rando

Post by Rando »

Okay, so now to your detailed toolpath-style question.

"...something that works on 5 by 5 block taking little off at a time on each stepover starting from outside working in to 2" diameter circle."

There are a couple things to unpack here:

First, the kind of toolpath you're thinking about is sometimes called a "trim to stock" toolpath. However, these are often very primitive because they are calculated offsets from the original toolpath, and assume the cutting parameters are okay in each of those. They tend to be less efficient than a more-traditional pocketing toolpath where the outside of the part is set as the outside of the pocket, the hole in the middle of which is the boss. For example, in this case, all the toolpaths would be concentric circles, mimicking the boss, and ultimately having a lot of air-cutting time.

Second, it really doesn't matter whether it starts inside or outside. Once the bit is down at depth, it's only cutting the step-over amount anyway. Thus, whether it's cutting "from" the inside or the outside only matters when it's a sloped surface and you're using a ball end-mill. In those instances, because you want to avoid center-cutting, you move "up" from the lower passes when doing that. So, as long as you're properly ramping into the material, and your other cuts are safe, whether it starts at the inside or outside usually won't matter.

And last, that's definitely the kind of thing a High Speed Machining pattern will do awesome at. They're fun to watch too, with all the non-rectalinear movements. And, because the stepover for HSM is always tiny (think 2-8% typically), you can run them FAST and the cuts DEEP. I'm regularly doing 0.30" deep cuts at 80 IPM in aluminum, but with only stepover in the range of 0.015". Fun as heck to watch!

Okay, I think I've about related what I know :D
=====================================================
ThomR.com Creative tools and photographic art
A proud member of the Pacific Northwest CNC Club (now on Facebook)

Post Reply