How to Set Up a 5 Axis CNC Machine | DVF 5000 | DN Solutions
6 Video Views·Sep 30, 2024
Architecture & Engineering
You ready to learn 5-axis?
All right, so we got our WD-40. We're going to put a nice light coat across the table.
So this is our stone. We're going to start out with our coarse side first and go in a figure
eight pattern. Make sure you're going to keep even pressure on this stone at all times.
Now as I'm going around this, I'm kind of feeling to make sure that I don't feel any like burrs or
anything sticking up, anything that the stone might catch on. If it does, then I know I have
a problem and I need to focus on that area more. And as I'm going around this, this table feels
really good. I don't feel any catches, so I'm not going to stone it more than I need to.
So now we're finished with the coarse side. Now I'm going to run back across it with the
fine side of the stone. All right, so we're going to move in that same figure eight pattern,
still feeling if we can feel any burrs, any kind of catches on this stone.
All right, so now I got the table stone. Now we're going to come in with a clean
towel and wipe it clean. I like to do small sections at a time and then moving my towel
around to make sure I got a clean portion of the towel, just to make sure I get up all of that
grit that was left behind from the stone. Well, now that I got the whole table done,
I'm going to go to a clean side of my towel again and go back over everything.
Now our table's clean and we're ready to mount our vice to the table.
So if you're still following along and you want to know where you can find more, then check out
academy.titansandcnc.com. Then scroll down to the Titan 5-Axis Series. Once you click on that,
the very first part you'll see is the Titan 139M. You'll click on that and then you'll see all three
videos for this series. This series is designed to go in sequential order. First, you'll start
with the CAD where you'll design this exact model. Then you'll step over to the CAM tutorial where
you'll program your part. And lastly is the CNC tutorial where you'll put it on the machine.
It's actually this video you're watching right now. This series is going to give you everything
you need from the print, the setup sheet, the tool library, and even the fixture model. Once
you complete each tutorial, you can go over to CNCexpert.com and submit your file to get certified.
This is fantastic because there's nowhere else that is offering certifications like this. And
the best part, it's completely free. All right, let's get back to the video. Before we mount our
vice to the table, we need to know what vice to mount. Well, if I'll take a look at the setup
sheet, I can see that the programmer has specified that we use the Contek KSC125 Centric vice
mounted on an SKQ125-1 riser. Now this is very important because the programmer has specified
what we need to use. So that's telling me that he's done the simulations and that if I use this
exact setup, we should be safe to run. Good documentation is paramount and key to success
in 5-axis machining. So here's our vice mounted on the riser as specified on the setup sheet. So
now we're going to flip this over, make sure the bottom is clean, then we're going to set it on the
table. All right, let's pause right here because there's a couple things that you've got to
understand. There's a couple different ways that you can program a 5-axis machine. We're going to
be teaching you the easiest way, which is using Tilted Workplane. Or if you're on a machine like
a Haas, you may be using Dynamic Work Offsets. Now those two codes are vastly different, but
essentially they do the same thing. We'll be explaining them in a different video, but for now
what you need to understand is that those codes allow us to put this vice and our work offset
wherever we want on the table. And we can run one program when we do that. If we did not have those
codes, we would have to program from the theoretical center line of the machine, or some
people call it kinematic center. If we did that, then our work offset would have to be at this
theoretical pivot point of where the table rotates, and we could never move it. Also, if we program
that way, our fixture and the material would have to be dead center of the table. And even worse,
the stack up from the fixture and the material would have to match our cam software perfectly.
If there was any deviation in that, we would have to go back to our cam software, repost it,
and then run a new program. We're not going to do that. That's old. It's outdated. We are going to
use Tilted Workplane or Dynamic Fixture Offsets. It's going to allow us to put this wherever we
want. Before you go any further, if this is your first time running any 5-axis machine,
there's two questions that you need to answer. Number one, is your cam software outputting
Tilted Workplane or Dynamic Fixture Offsets? Ask your reseller. And number two, is your machine
already set up with those codes ready to go? Most new machines are already set up this way.
The person that installed your machine comes in and they get that set up for you, but it's a good
question to answer before you get started. Now that we know that, let's go ahead and get this
vice set up. I'm just going to eyeball it to the center, and then we're going to put our bolts in.
So we got it pretty close to the center here. That looks good. Now I'm going to get my T-nuts
and my bolts. Here's our bolt and our T-nuts. Insert this T-nut in here.
All right. Now we put our second one in. T-nut, bolt. Now here's the part I love about 5-axis.
We can go ahead and tighten our bolts. We don't have to knock anything around,
because we got a C-axis. We can just adjust it to line the vice up. So we're going to go ahead
and tighten our bolts in now. Now step one is complete. We've got our vice installed in the
machine. Now let's move on to step two, where we install the tools. So if we look at the tool list
on our setup sheet, you'll see that tool one is a three-inch face mill mounted on a two-inch long
face mill arbor. Now this is an eccentric tool, meaning we can't touch off on the center.
So we're going to need to know roughly what the length is before we put it in the machine.
So we've got a set of calipers here. We're just going to measure out roughly that length to the
gauge line, and I can see that's around four inches. So we're going to put that in when we
touch the tool off. So first I need to call up my tool one at the machine. First we're going to
close the door. Now on our control, we're going to go to MDI. We're going to go to program. Now we see
our MDI screen here. We're going to type in T1M6 end of block insert. Now we see that's inserted
here. Now we're going to just hit cycle start. All right, tool one's in the spindle. Now we can
hit our door open request, open our door, and we're going to put it in handwheel mode
and jog the spindle over to where I can reach it.
We'll hold our tool unclamp. We can insert it in the machine,
hold our tool unclamp again, and it's locked in. All right, now we're going to close our door again.
Now to touch this off, we're going to go to our GUI screen, and you might get this screen pop up.
This is just telling you you have to hit reset first. So if we hit our reset, go back. We reset.
Now we're going to hit GUI. Now we're going to do tool set length. For cycle type, we're going
to leave it at automatic. Tool type, we're going to arrow over to off center. I'm going to arrow
down to tool number one, or we're going to type in tool one. All right, now tool diameter is three
inches input, and our tool length is incorrect. It took that from whatever is saved in the tool
offset. So we need to highlight that and input four inches. Now we can go to our memory and hit
cycle start. It's going to come down and touch, back off. Now we look at our screen and we see
that this is the measurement it took. The length is actually 3.9718. All right, now we're going to
repeat the process for tool two and tool three. So we're going to go to our MDI, go to program,
make sure everything is reset, and hit T2, M6, end of block, insert, and hit cycle start.
All right, looking at our setup sheet, our tool two is a quarter inch chamfer
mounted in an ER16 by four inch long holder. Insert the tool. Tool two is in the spindle,
so let's go ahead and close our door. All right, before we go to our GUI, make sure we hit reset.
Now go to GUI, tool set, length. Now this time we're going to use on center. We don't have to
know the tool length for on center tools. All we have to input is the tool number, which is tool
two, input. We'll go to memory and hit cycle start. All right, now we see that that measured
length is actually 4.7677. All right, now we need to call up tool three. So go to our program screen,
go to MDI, T3, M6, end of block, insert, and cycle start. So looking at our setup sheet,
tool three is a 116th ball nose end mill also mounted in an ER16 by four inch long holder.
Insert our tool. So this is going to be the same as tool two. Hit reset, GUI, tool set,
length. We'll go, it's going to be on center. This is a ball nose. It's going to be tool three,
input. Now we can just go to memory mode and hit cycle start.
Measurement on that's done. We see the length is 4.5172. Now the last thing I like to do
is actually go to the offset page, look at my tools, make sure the numbers are correct,
but also look at my wear for each of the tools that I'm going to be using for the length and
the radius to make sure that there's no numbers left in there that might be comping the tool that
I'm not aware of. So we see that all of these are zero. That's good. That's what I want. Step two
is complete. We got our tools in the machine. Now let's go to step three, where we put our material
in the vice and get it touched off. Now, before we put our material in the vice, we need to set
our G54C0. And to do that, we're going to take our indicator and indicate along the back jaw of the
vice. So let's do that now. Indicator on the spindle, just bring it down so we can indicate our vice.
Now this is a centric vice, meaning both front and back jaws move, but this shunk vice is pretty
tight and I'm not really worried about any slop in it. So I'm going to go ahead and indicate off
this back jaw. So I'm just going to move my indicator down. All right, I'm going to show
you guys a really quick way to indicate a vice on a five axis. So normally when you're indicating
a vice in, you would zero your indicator on one side, go all the way to the other side and see
what the difference is, and then cut it in half and move by that amount. But on a five axis, we can do
this much quicker if we start in the center, where this is the actual pivot point, zero indicator
right here, and then just move to one side. And I'll show you how we're going to do it.
All right, so we're going to zero our indicator. All right, now we're going to move in X all the
way to one side so we can see the indicator doesn't even touch. So now we're just going to
move in C until we're zero on our indicator. So I'm going to rotate my C. All right, now it's zero here.
Now let's go all the way to the other side and see what we get. Put it in X. Now you can see
we're zero all the way across. Super quick. All right, now we're going to go and set our G54 C0.
All right, to set our C0, we're going to go to offset, come up here to work. We're going to arrow
over to our G54 here, come down to C, and we are at C0. We're going to hit measure.
Now you see that number populate here, and our absolute coordinate system here, it zeroed it out.
So now that we got C set, now we can go put our material in the vice and get our X, Y, and Z set.
Now this is very important right here. This B always needs to be zero. If your vice or whatever
fixture you're using is not flat with the table, then you need to go in and adjust it to make it
flat. Shim it, recut it, do whatever you need to do, but do not put a number in this B axis offset.
We'll go over that later down the road why you can't, but just know that it won't calculate
correctly if you have a number here. All right, so with that, let's get our material put in our vice.
So now that we've set the C axis work offset, we can now install our material into the vice.
And if we look at the setup sheet, it says to clamp the part in the center of the vice using
the serrated teeth at three millimeters deep, and then torque to 50 foot pounds. So let's do that now.
Set it in the center of our vice. I've got my caliper measured out. All right, now let's get
our torque wrench and torque it to 50 foot pounds. Now we may want to make more than one of these,
so I'm going to set up a vice stop on the left side of my vice. And keep in mind, a lot of the
things that I'm using in this video, you can find on our online store. Tag it to the left side of my
vice, come over till it touches my material, and tighten it down. Now I want to make sure that this
stop isn't sticking out too far above my jaws so I don't hit it. So there's one more final
verification that we need to make. And looking at the setup sheet, it says that the material should
stick out above the top of the vice 2.880 minimum. So let's check that now. All right, so we're at
2.950, so that's plenty good. Now we're ready to call our probe up and teach our X, Y, and Z offset.
Close our door. All right, so we're going to go to MDI. We'll hit program. And my probe is tool 60,
so I'm going to type in T60M6 endoblock insert. All right, now I see that's called up. Now I'm
just going to hit cycle start. All right, now we're going to put it in hand jog mode. I'm going to move
the probe over to the center of the part. I'm just going to roughly eyeball it here. All right, let's
find our X first. Let's make sure you hit reset. You know, you got to hit it four or five times.
You can't just hit reset once. Let's go to GUI, and this time we're going to select probe.
Probe. We're going to do a web. All right, now we see we can do an X web first.
What the work offset is, we're going to put 54 input. The width is going to be the width of your
material. So we're going to put 2.25 input, and we're going to use a depth here. This is how far
it's going to move incrementally from where it's sitting now. So I'm just going to put in, you know,
maybe 0.6. Hit input. So now everything's input. Now we're going to go to memory
and hit cycle start, and that's going to pick up our X, G54. All right, now the X is set to the
center of the part. Now let's find Y. So we're going to move this to just hit our over arrow to
Y web. Now we're going to come down the same thing. G54. Our width is two and a quarter
input, and depth, we're going to use that 0.6 again. All right, now that's set. We're still
in memory. Now let's hit cycle start. It's going to pick up Y. All right, now our X and Y zero is
set to the center of the part per the setup sheet. Now we look to see that Z is set 20 thousandths
from the top of the stock. We're going to touch a single edge this time. Make sure we hit reset.
We'll hit our back arrow, and we're just going to do Z negative here. Z negative. Now here all
we need to do is tell it what work offset. So we're going to put in 54 and input. Now whatever
it touches, it's going to automatically set that at zero. So now we're going to make sure we're in
memory, and then we're going to hit cycle start. All right, now it's set our G54 Z zero, but it's
set Z zero off the top of the part, and on the setup sheet we need to be negative 20 thousandths.
So let's go to the offset screen. We'll arrow up to our Z, and we'll type in minus 20 thousandths,
and hit input plus. That's going to say, is this number okay? We're just going to hit execute.
All right, now that we have X, Y, Z, and C set on our G54 work offset, now we're going to load our
programs on our machine, and there's a few different ways you can do this. Number one,
you could have your machine hooked up to a network and send the program straight to it
from your computer, or you can use a USB drive. What we're going to use today is an actual compact
flash. So we're going to insert that in right here on the top, just like that. So now we got
our memory card installed. We're going to go to edit, go to our program screen. Now we make sure
that our folder is selected here. Now you're looking at all the programs I have stored in
my memory of the machine. Next we need to go to device change, and I'm going to select my memory
card. Now this is all the programs I have on this card, which is the Titan 139M, OP1, and OP2. So
I'm going to copy both of these programs into my memory side. So I'm going to select both of them
at the same time. So how we do that is we're going to hit the right over arrow, and I'm going to
highlight both of these. So I'm going to hit select, and the arrow down to this one, hit select
again. Now both are selected. I'm just going to hit copy. Now we're going to right arrow again
two times to where we see device change. Now we'll hit that, and we'll hit CNC memory. Now I'm back
on the machine side. So here I'm just going to hit the right arrow again and hit paste.
Now you see both programs get brought in to the machine side. All right, now we're going to arrow
down to our OP1 program, and I'm going to hit the right arrow twice, and I'm going to select this
main program button. Now you see this little at symbol highlighted our OP1 program. That lets me
know that it is the main program. So now I can go to a program right here on the top right
and see my program. Now all we have to do is select our memory,
and we're ready to hit cycle start and run our program.
Start out by facing the 20 thousandths off the top. Now we're going to rotate over 90 degrees.
It's going to come in and face our sides. That's that roughing and then the finishing pass,
and we'll repeat that for all four sides. All right, now with that last side done,
our face mill is complete. Now we're going to come in and chamfer the part.
With this last side, then all five sides have been chamfered.
Now we're going to come in and start engraving. We'll start with the top side first.
That's going to rotate down and engrave our eagle on the sides.
That's the last side. All right, with that, OP1 is complete. Now we're going to take it out
and flip it over and reteach everything and then run OP2. But before we put it back in,
the setup sheet says that Z0 is on the bottom of the part, which is the bottom of the vise.
So we're actually going to probe the vise first before we put the part in.
All right, I'm just going to set it to the side. We're going to go and call our probe up,
probe the bottom of the vise, but before we do that, we need to make
extremely sure that B is at B0. We don't want the table up at any angle when we set our work offset.
In OP1, we're going to probe Z, but in this case, our Z0 is on the bottom of the vise.
So after that teaches the Z, now we're going to move up and install our material.
All right, so we're going to follow our setup sheet,
holding the part all the way in the bottom of the vise and right in the center. Now we can tighten
and torque it down. Now we've got our part set up and tightened. We can go ahead and install our
stop. Now we can come back in and probe X and Y, just like we did in OP1. All right, one thing to
note is I am probing on the raw stock to begin, which is not a good thing to do when you're
holding on a finished part. So what am I going to do is when we're running the program, after
the face mill runs, this excess stock is going to get removed. Then we're going to stop the machine
and re-probe on our finished size. All right, now our X, Y, and Z is set. Now we can run our OP2
program. All right, now that we got that excess stock gone, we're going to come back and re-probe
it on our finished part. Now that we've retouched everything, we're going to continue on in our
fundamental part to learn five axis on. Thank y'all for watching. Look, this is what we do.
This is what we're all about. So if you want to support education just like this,
then hit that like and subscribe button. We'll see y'all next time. I'm going to the academy.

