Download the Kennametal Tool List and check out the FREE Academy Resources for this project in related files to the right of the video tutorial: https://academy.titansofcnc.com/serie...
This tutorial provides a comprehensive guide to programming the Titan 1M part using Mastercam on a Haas three-axis mill. It covers the entire workflow from initial setup and stock modeling to advanced roughing, finishing, chamfering, and tapping operations, emphasizing safety, toolpath verification, and the conceptual differences between 2D and 3D machining.
Hey, what's up everybody?
This is Titan, Titans of CNC, and today I'm going to teach you how to program the Titan
1M in Mastercam.
Alright, so before we get started, let's just talk about a few things that you're going
to need.
Okay?
Here is the print.
It's a three-part print.
This is the exact same print we used in our last video when we taught you how to design
the Titan 1M.
You'll need the setup sheet with all five tools and instructions, and then you'll need
to download and then upload all 16 tools in the Building Blocks Toolkit.
Alright?
All documents and links are in related files attached to the Titan 1M project.
Are you guys ready to learn some crazy Mastercam programming skills?
Let's go.
Alright, so let's get started.
I'm going to step up to machine.
I'm going to go pick out what machine I'm actually going to CNC machine this part on,
and that would be our generic Haas three-axis mill.
Boom.
Alright?
Now, here's something cool.
I'm going to teach you 2D toolpaths and some 3D, and the difference is the 2D will basically
offset from these simple lines, and it won't have a brain, meaning it doesn't understand
the part that it's machining.
A 2D path simply knows that you told it to offset off a particular line, feature, contour,
etc.
Alright?
But a 3D toolpath reads the model.
A 3D toolpath has the ability to understand and read off of the raw bar stock that you're
cutting the material from.
Alright?
And when one tool comes in and cuts part of the material away, another tool can come in
and understand that part of the material was taken away, but there's still material in
the corners.
So let's not waste time.
Let's drop into where the material has been removed and simply cut what was left over
from the previous operation.
Alright?
We call that rest machining.
Alright, let me stop there because I don't want to confuse you.
I just gave you a little taste.
Alright, so to build the stock around the part, I'm simply going to go over to wireframe.
I'm going to hit bounding box.
Boom.
Okay?
Now I'm just going to click this guy and I'm going to say end selection.
Oh, look at that.
Looks great, right?
When I look at my setup sheet, I can clearly see at the top it says 1x2 bar stock cut 4.1.
Alright?
So we're going to duplicate that minus the top material.
Okay?
So basically, we're going to put all the material around the outside, which is going to leave
the material on the inside.
We're going to put the material on the bottom just because the 20 thousandths per our setup
sheet that I'm going to cut off the top is going to be done with a 2D path and therefore
it's not going to read the material because when I bring up tool 2 to actually do the
OptiRough path, it's just not going to care about the top because tool 1 would have already
faced it.
Alright?
So anyway, I don't want to confuse you.
So let's just move forward.
So we're going to come over here, lock this guy down 4.1, boom, alright?
Now we're going to go 2 inches, boom, alright?
Now you can see the material all the way around the part and now we're simply going to add
the material to the bottom, okay?
So now I'm going to just click here, kind of just to show you guys, right?
I don't actually need the material on the bottom but I'm just going to show you how
I would put the material there if I needed it, okay?
So I'm going to grab this guy, look at that, so we can just bring it down.
Now I'm going to go 0.23, okay?
So 0.23, enter, enter, okay?
And now when you actually look at the size, it's 2 inches by 4.1 per the print and then
it's 980 which is 20 thousandths shy of the 1 inch, alright?
And if you're wondering about the 20 thousandths, I didn't put it there because on our operation
setup sheet, if you go to the bottom, it says Z axis top of part and it says drop negative
20 thousandths for facing.
So I'm basically with tool 1, I'm just going to face that off, it's a 2D path, it wouldn't
read the material anyway, so since I have experience, I'm simply not going to add it.
And we are good, okay?
So I'm going to hit this guy here, boom, and there you go.
Alright, so now we can actually see that the raw material is over my part and I can't quite
get to my part, alright?
So let's take this new model and drop it to a different level, okay?
So I'm going to click this guy, then I'm going to come over, remember this from the last
video, I'm going to click select all wireframe, now I'm going to come over, I'm going to right
click and I'm going to drop it to a different level.
So I'm going to click here and then I'm going to change this, I'm going to unclick this
guy, I'm going to put 3 here, drop down, I'm going to name it stock solid and I'm going
to say okay, boom.
Now I'm going to come down to my levels and there you go, alright?
Now, okay, so now that we know how that works, let's actually go to the next step.
So I'm going to come up to toolpaths and then I'm going to call this model a stock model
by hitting here.
So I'm going to say stock model, I'm going to name it stock model, now I'm going to select
it by hitting here, grabbing it and hitting end selection and then I'm going to hit the
check, boom, okay?
Now I'm going to turn this guy off and you can see that the stock model is basically
in the same position as the original model that I created with the bounding box.
Alright, so now that we have our material, let's actually do a little bit more housekeeping.
I'm going to go to tool manager and then I'm going to open this folder right here and then
I'm going to grab the building blocks tool list and there's my 16 tools for the building
blocks, alright?
So as I said in the beginning of this video, it's important to grab this tool list from
our academy, it's a free download, so grab it now and place it here before you continue.
Alright so now I'm going to look at my setup sheet and I'm going to simply pick the five
tools that I'm using for this operation, alright?
I'm going to grab this guy, bring it over, face mill, tool number one, okay?
Second tool is a 3 8's, boom.
Now we're going to grab our quarter inch chamfer, which is tool three, boom, and then we're
going to grab our .177 drill because we're doing a 10 32 roll tap, I'm going to grab
this guy, bring it in, then we're going to grab our 10 32 tap, boom, and there you go,
our five tools.
As I move forward programming with these five tools, I'll change the tool number so it reflects
one, two, three, four, five.
Alright so we're all set.
Alright so let's program tool number one.
I'm going to go over to our tool paths so I can see everything, you see our stock is
right there, and I'm going to go up to face, alright?
I'm going to go to my setup sheet, tool one is a three inch face mill, so I'm simply going
to come up here, I'm going to say face, now you can see the tool path populated and instantly
there's a box saying solid chaining.
So what it needs me to do is select the surface that I want to face, alright?
So to make this easy, I'm going to drop down here, I'm going to hit levels, I'm going to
turn my stock model back on, and therefore I can select the entire surface going around,
okay?
So I'm going to actually click this side, boom, and you can see that the entire box
is now a chain.
And now we see this box right here, so I'm going to say okay by checking it, now I'm
going to click down here, I'm going to say yep, that's exactly what I want to cut, boom.
And now it's time to fill out all the information for the tool, okay?
So we can see that facing is highlighted, our geometry is one because we've picked the
one surface, we're going to go into tools, I'm going to select my one inch face mill,
I'm going to double check and make sure that my tool number and offsets are correct, and
then make a few changes down here, alright?
So spindle speed, I'll go 4,000, just to be safe because we have a lot of students and
first time machinists following this video, we're going to keep our RPMs nice and low,
okay?
So 4,000 RPMs and below.
Change my feed rate, I'll go 25 inches per minute.
Plunge rate will be 100 inches per minute.
And go to holder, I don't really care, so I'm going to come over here to cut parameters,
and because we're dealing with a 3 inch cutter and the surface across is only 2 inches, I'm
going to change this guy to one pass.
I want to go right down the center, you can see the green line right there, boom.
Right down the center, and now on our overlap, I'm going to put 120, I'm going to put 120%,
which is going to allow us to start on this side off of the material and end on this side
off of the material so that we don't leave any tool marks, alright?
Now over here, I'm going to just zero these guys out and we're good.
So I'm going to go to cut depths.
This is if we're doing multiple passes and we're not, okay?
So let's just go to linking.
Now this is important, okay?
So we're going to hit our clearance, which is our initial plane where we drop down to
at the beginning.
I'm going to say 2 inches, that's fine.
I'm going to say only raise or fall to this position at the start and end of the program,
alright?
That's a safety thing right there, okay?
Our retract is good at a quarter inch, 0.25, and then our feed plane we'll keep at 0.2,
which basically dictates when it starts feeding in Z, alright?
I'm going to hit this guy right here and keep it absolute, okay?
Actually I'm just going to go down and hit absolute all the way across.
Whenever dealing with students, I like to start off with absolutes so we know exactly
where we're at, alright?
And that's why we've also kept our Z zero at the top of the part.
That means everything above it is positive, everything below it is negative.
When looking at code, it's just an easy way to know when you're engaged, when you're in
danger, meaning when you're underwater, or if you're in the air and it just doesn't care.
It's like a rap song, right?
But it's true.
If this is Z zero, when we're up here, we're flying around, we have no cares in the world.
This could be the ocean right here, but as soon as we drop below Z zero, it's like bloop,
bloop, bloop, right?
This is negative.
Now, this is material.
This is danger.
You have to understand that at that point, you're either cutting material or you're in
a pocket that if you move across, you'll actually scrap the part and crash the machine and we
don't want to do that.
Alright, so there's the reason behind our Z at the top of the part and keeping everything
in absolute.
So top of stock is 20 thousandths, boom, that's up there.
Our depth of cut is right at zero, right across that surface and we're good, okay?
You can come down here, doesn't really matter, doesn't matter, doesn't matter.
I can take the coolant here, I can actually turn it on, boom, and we're good, alright?
So let's just click this guy and there you go, alright?
So that's the tool path.
We're going to drop down and go up, okay?
So I'll go over here, tool paths, you'll see it right here.
Now check this out.
I can actually click up here and it shows you the tools, alright?
That's back plotting.
So I can actually hit the play button, it'll show the tool, come down or I can stop.
Now watch this.
I'm going to hit that S key, take a look at it, make sure that you're perfect, alright?
And you can hit S again.
Oh, we're way over there.
What if I actually want to back up?
Hit the B key, boom, alright?
So it's like boom, boom, boom, boom, ah, okay, there you go.
S and B key moves it forward and backwards and here's something else.
If you hit this guy right here, you can actually come in and say interpolate and then you can
set your step increment.
So we'll go 0.2.
Now say okay, I'll restart it.
Now watch, I stopped it, S, it just goes 0.2, boom.
Cool little trick, right?
If I want to back up, I can just back it up, I can move forward, I can double check everything
and I'm teaching you this right now because back plotting is incredibly important and
it is how you can ensure that your tool path is actually great.
And this is great because we want to actually proof out the tools right here, we want to
have a clear understanding of what they're going to do right here in Mastercam, not when
we're on the machine, alright?
So I'm just going to okay that and there's our first tool path.
Alright, so now that our facing operation is complete, let's go ahead and move on to
the next step, alright?
So I'm actually looking at my model and I can see the material around it and I can see
that if I actually step up here and hit that guy, it gets dark, right?
So that tells me that my other level is turned on, so I'm going to go ahead and turn it off
there, see, boom, boom.
The only reason I turned that one on was that it allowed me to actually click the entire
top surface for my face cut, alright?
Now the only thing I have to worry about is my stock model, which is right here and we're
actually going to use it in the next tool path, which is OptiRough, okay?
So alright, I actually want to get rid of that tool path, so I'm going to come over
here, click that, boom, it's gone.
Alright before we get to the OptiRough, I'm going to go ahead and right click, I'm going
to say top, boom, I'm going to push away.
Now for OptiRough, I actually have to have a boundary, okay?
So I'm going to actually create a boundary around the part and an easy way to do that
is simply going to wireframe, circle, I'll click here, pull it out, move away, pull it
out and I'll click, okay?
Now I've got this nice big diameter right here, I'm going to go ahead and click right
there, boom, accept it, alright?
And now that will be a containment boundary for my tool path in OptiRough.
So I'm going to go back to tool paths, I'm going to go to OptiRough right here, boom,
everything pops up, tool path, OptiRough, it's already highlighted, I'm going to go
to geometry right here and I'm simply going to click over here, boom, and then I'm going
to click the model.
If I click one time, it'll be this surface.
What I need to do is click it three times in a row to click the entire model.
So I'm going to click one, two, three, boom, okay?
Now I'm going to say end selection, so we're good, boom.
Now when you look at this section and this section, this is the wall stock, meaning the
wall stock here, this is the floor stock, the floor would be down in the pocket or on
the top, over here, that's all the floors, okay?
And it's basically asking me, do you want to leave material on there?
And since it's a roughing operation and because I'm going to come back and clean it up with
a finish pass, then I will take advantage of it, but let's actually do five thousandths,
okay?
Five thousandths per surface, .005, .005, now I'm leaving five thousandths on the walls,
five thousandths on the floor, and that's it, okay?
This box over here, just for reference, just for future knowledge, this is avoidance, alright?
So just like I clicked the model as my machining geometry, if I actually had a vise attached
to it or work holding or I had anything that I did not want to touch, I would simply hit
this guy, click it, it would rise up over here and I would say how far do I actually
want to stay away from it, quarter inch, half inch, whatever it is, I would put it right
there and then it would make sure that the tool path stayed away from that vise or that
work holding, okay?
So moving forward, now we're going to go to boundaries and guess what?
We have a boundary, so let's click this, my solid chaining box comes up, so I'm going
to switch over to wireframe, then I'm going to click this guy, boom, and that's all I
need.
So I'm going to hit the check, there you go.
So I'll say inside, center, boom, that looks good.
I'm going to go to my 3 8ths flat end mill, I'm going to say this is tool 2, my feed rate
will be 25 inches per minute, plunge rate will be 50 inches per minute, spindle speed
4,000, again keeping it nice and slow for training purposes.
Retrack rate, it's rapid retract so it really doesn't matter.
We don't care about this guy, but we do care about this, okay?
So now rest material would be the amount of material that we have left on the part and
we know that we have quite a bit of material, right?
So it's 1 by 2 by 4.1, okay?
We took a face off the top, so Z zero, the top of the part is perfect now.
So basically we just need to come in, hog out this pocket, hog out this pocket and go
around the part, okay?
So I'm going to hit rest material, now I'm going to click here, one other operation and
check it out.
It went to stock model.
So I'm basically saying we're going to take off the material from this other operation
right here.
Make sense?
All right, so now we're going to go to cut parameters, we're climb cutting at 25 inches
a minute, our tip compensation is at tip, we're going depth, material and all of that
is perfect.
On my step over, I'm actually going to go 15%.
All right, so our step down is going to be 200%, which is 750, we're going to click step
up.
Then my step up, I'm just going to put in 50 thousandths.
Now what I know is there's no slopes, all right?
If there was a slope, it would make a bunch of passes 50 thousandths up, okay?
But here I could really put 50, I could put 250, 200, it really doesn't matter too much
because once it reaches this level, it's going to cut this level, cut this level, leaving
the five thousandths that we left in geometry as far as on the walls and the floor, et cetera,
right?
So we're going to say 50 thousandths, this guy we're going to say 20 thousandths, lift
height, that'll be every time it cuts and actually comes back, you can see it right
there, it's going to be at 10 thousandths, that's perfect.
Back feed rate is at 100, which is also great.
Now I'm going to go to transitions, all right?
So on my helix radius, I'm going to come in here, I'm just going to make this 150, boom,
that'll make it a diameter of 300 thousandths, Z.1 is fine, plunge angle is 2 degrees, leave
that alone and we're skipping any pockets that are less than 0.55, I only have a few,
so we'll leave that alone also.
What I will change is this guy because our standard feed rate is at 25 inches per minute
but I want to slow it down because our standard feed rate is 25 inches a minute and I want
to slow it down when ramping.
So I'm going to take this, I'm going to actually go down to 15 inches per minute, I'll leave
ramping speed at 4000 and this would allow us to dwell at the bottom before we get into
the material but I'm going to leave that at 0.
Now steep shallow, I'm going to click this guy right here and that says adjust for stock
to leave, which in the geometry, I left the stock here and we want that stock to be left
so we're clicking this guy so it reads the other one.
Alright, makes sense?
Now I'm going to click this guy, leave this at 0, I'm going to click this maximum depth
and then actually over here, I'll just put negative 0.750.
Now we'll go to linking parameters, I'll leave this guy at 2 inches, absolute, full retract
every single time, I'm going to leave that alone, I'm going to drop down, 25, vertical
entry 75, 75, 75, 75, all looks perfect, ramp height 100, boom, love it all, then I'm going
to come here, we're good, we're good, coolant, let's turn the coolant on, boom, we're good,
let's try out the path.
Alright, so this path looks absolutely fantastic, I'm going to go ahead and back plot it, toolpaths
looking really good.
You know when you guys have a lot of experience and depending on the type of tool you're using,
these step overs, which are just about 15%, you can actually increase those depending
on your depth of cut and the ability of your end mill, alright, 15% was just safe, and
therefore that's the number I used.
Alright, so next thing we're going to do is actually finish the outside, finish this step
right here, and finish the pocket.
To do that, we're going to use the exact same end mill, tool number 2, we're going to hit
contour, and boom, you see contour pops right down here, and then we're ready to create
our chain.
I'm going to start it right here, I'm going to actually click this guy right here, unclick
here, press shift, boom, and there you go, all the way around, okay?
Looks really good, alright?
I clicked the top here because the bottom was actually the bottom of the chamfer and
it was not the outside of the part, see?
So I actually clicked the top line so I could ensure that I was on the outside of the part,
therefore our finished pass will be perfect, okay?
So I'm going to okay this, alright, so we're at contour, our tool is tool number 2, because
we're in a different tool path, our RPMs have changed, so I'm going to actually put 4000
here, and I'm going to change my feed rate, I'm just going to go 20 inches per minute,
nice and slow, 100 inches per minute on the plunge, retract, we're just going to say rapid
retract, and that looks good, come over here, looks good, cut parameters, I'm going to actually
turn on cutter comp, so I'll hit this guy, I'll go to wear, tip, everything here looks
good, cut depths, it's fine because we're going to one depth only, lead ins, I'll go
ahead and leave this alone, right here, everything looks really good, breakthrough doesn't matter,
multi passes does not matter, taps, linking, alright, so I'm going to go ahead and turn
back on our clearance, I want to make sure that it's just at the beginning, it really
doesn't matter, but I'm just going to click that guy right there, we're going to keep
on absolute throughout, so absolute, absolute, absolute, retract is quarter of an inch, B
plane is .2, top of stock is zero, depth is zero, so we're actually going to drop down
to negative .760, we're just going to overshoot the part, the part is .750 thick, or three
quarters of an inch, we're going to overtake it by ten thousandths, just to make sure that
the entire surface that we cut is beautiful, there we go, everything else is looking good,
coolant, I'll go ahead and turn on, and there we go, alright, so let me actually show you
something right here, I don't want it to start in the center right here, okay, so I'm actually
going to go back and change that, so I'm going to go into parameters, I'm going to go into
my lead in, lead out, and see this guy right here, enter, exit, midpoint, I'm going to
uncheck that, now I'm going to okay it, now I'm going to grab it again, boom, alright,
so now it started at the beginning of the chain, hit this guy, and there you go, that's
the pass, nice and perfect, everything looks good, alright, so let's go do the next pass
and that will be finishing this step right here, this surface on the bottom is a little
bit greater than the diameter of the tool, so I'm actually going to have to make two
cuts coming in to make sure that I get everything, okay, so let's go, I'm going to hit contour,
I'm going to come down here, now when creating the chain, you can see that the chain here
kind of dips in a way, right, it actually won't matter too much, but let's actually
go up here, okay, because once I put the depth, it will all work itself out, okay, so I'm
going to hit this guy right here, now, here's another little trick, see this, this little
pointer right here takes the X forward, this one goes backwards, so I'm going to go forward,
forward, forward, forward, and then that's the exact chain that I want, so I'm going
to hit the check mark, now, since we're using the same contour pass that we did previously,
our tool 2 and the speeds and feeds should be the same, which they are, so I'm going
to just simply move ahead, come to cut parameters, the wear is the same, everything here looks
good, I'm going to drop down to depth of cuts, I'm going to go lead ends, that all
looks good, now, where it's going to change is here, multiple passes, I'm going to click
this guy, I'm not going to worry about roughing, I'm going to come to finishing, I'm going
to say 2 passes, my spacing is going to be .200, and then I'm going to move forward,
I'm going to say final depth, and then I'm going to say keep tool down, so when it roughs
here it just moves over instead of raising up and coming down, I'm outside of the part
so I have confidence and that will work, okay, now we're going to go to linking parameters,
and then I'm going to put in negative .5 for my depth, I'm going to say okay, and there
you go. Alright, so our next tool path, we're going to actually go up to 2D, drop this box
down, I'm going to hit pocket, now I'm going to simply click right inside of here on the
bottom of my pocket, let me switch it around so we can see it a little bit better, I'm
going to hit this guy right here, hold in shift, boom, alright, and that is exactly
what I want to cut, okay, so I'm going to okay it, my box comes up, now let's just simply
go through the tabs, there's my tool 2, that's what I want, I'm going to come over here,
change my RPMs, I'm going to go here, 20 inches per minute, boom, plunge rate is 100, and
the retract will be rapid. Alright, so that looks good, now one thing that I'll say is
plunging straight down into a finish pass is not smart, but I'm going to do something
a little bit different and explain it, okay, so just stay with me. So holder, we're fine,
cutting parameters, we're climb milling, the pocket type is standard, tip, we're fine,
sharp, down here we're going to get rid of these guys, just put it at 0, boom, now that
all looks good, go to roughing, our cutting method, there's actually a lot of different
choices here, okay, but we're going to hit parallel spiral, 50% step over is good, distance,
boom, everything looks good, entry motion, I'm just going to switch it up a little bit,
I'll go 45 here, a little bit smaller, over here, it says maximum, I'm just going to go
50, Z clearance, where I start, I'm just going to say 20 thousandths, 100 thousandths off
the wall, sounds good to me, plunge angle, we'll put 2 degrees, tolerance, 5 thousandths,
that's all fine, and there you go. So now we'll go over to finish, make a couple adjustments,
my spacing for my finish is going to be 5 thousandths, compensation is going to be where,
and then we're only going to machine finish passes at final depth, alright, that's just
the outside diameter finish pass, and that just means it's going to actually cut the
bottom and then it's going to come in for one final finish pass on the outside, which
is exactly what we want. Unclick this guy, lead in, lead out, boom, boom, you know I
actually might change this a little bit, since we're down in a pocket, the line doesn't need
to be that long, so let's just make this very small, 50 thousandths, our radius, let's put
at .25, and then let's angle it at 45, helix height, let's just go maybe 20 thousandths,
and then just do the same thing over here, so we'll go .050, tap through, .25, 45, .02,
boom. Alright so, we'll bypass this guy, bypass this guy, go to linking parameters, now this
is where it's going to get a little tricky, okay, and a lot of people would not send you
down into the darkness, like I'm going to right now, but I'm going to explain it, okay,
so we're going to say clearance is at 2 inches, everything is absolute, we're up in the sky,
then we're submerged into the ocean, everything below zero, alright, you never want to rapid,
you never want to move fast when you're below zero, unless you're extremely confident, and
that's what I want to talk to you about, okay, so our feed plane is going to be negative
.4, our top of stock is going to be negative .4, and then our depth of cut is going to
be negative .5. Now, why did I do that? I did that because I am confident that I actually
came in and did an OptiRough pass, and actually cleaned everything out and only left enough
for a finish pass. When we run the part, we'll ensure that all the material is gone and therefore,
when I create my helical, I won't start at the top and waste a bunch of time dropping
to the bottom, I'll actually drop down negative 4 because there's no material there, and then
I'll start my helical down low, which will save a bunch of time, get me to the bottom,
and then I'll just take off the .005 that's on the floor and the walls, alright, does
that make sense? So, I rarely drop down below the top surface, but in this particular case,
because we know it's roughed out, we're going to do it. I'm going to come down here, I'm
just going to say, hey, let's make sure the coolant's on, boom, I'm going to say okay,
and there you go. Alright, so check this out, if I hadn't put that negative 4 on the feed,
we would be feeding from up here, like all the way down, okay? But instead, it drops
into space, drops down, gives you a nice path right to the bottom, and then it starts cleaning
up, alright? And over here, same thing, it goes up, goes over, drops down, and then it
radials into the cut, nice and perfect, looks beautiful, oh yeah, love it, love it. Alright,
so I'm going to, I'm actually going to save this, make sure we're good, and that's it,
like, that's it for like the hard stuff, now everything else is going to be easy, okay?
Really easy, so let's go ahead and just start finishing up. Alright, so the next thing we're
going to do is, we're going to actually create the chamfers going around the parts, we're
going to go out here, we're going to go in here, we're going to step down by this wall,
and go here, okay? And to do this, I'm going to show you two different deburr passes, or
chamfer passes, and just so you know. So first one, let's go back into our tool paths here,
go to contour, now let's select the contour that we want, so I'm going to select here,
hold down shift, now watch, I can hit this, or I can actually hit this guy, I'm just going
to say, yep, that's the direction, that's the direction, that looks perfect, boom. Alright,
so now before I hit the okay button, I want to explain something to you. There's already
a chamfer drawn here, so I actually went to the inside of the line, which kept me at the
top surface, and I know that if I say do a chamfer from this line, it will automatically
put the depth exactly where it's supposed to be, because I know that when we did the
last video, and I put the chamfers on, I did them at 10 thousandths per print, which is
perfect. I'm going to hit okay, I'm going to go through tool, I'm going to go down here
to my chamfer mill, I'm going to call it tool three, go down, now I'm going to go 25 inches
per minute, plunge is 100 inches per minute, holder is fine, cut parameters, now watch
this, 2D, click contour type, 2D chamfer, boom, okay, got my wear on, left, tip, boom,
all of this looks good, okay. Now here's the trick, because I went on the inside of a line,
I don't need to put a chamfer width, because it knows exactly what to do, because I went
on the inside, therefore at a 45, it will cut perfectly from that line, so I'm going
to hit this guy, zero, come down, now this is taking my tip and offsetting it off of
my part, and since I have a quarter inch tool, and half of that tool is an eighth of an inch
or 0.125, I'm going to go tip off at about 60 thousandths, okay, boom, and that looks
good. Now cut depths, I don't worry about lead in, lead out, everything looks pretty
good but we can tighten it up a little bit, so let's just go 0.05, let's go 0.1, we're
only doing a 10 thousandths chamfer, so a radius coming in at 100 thousandths is sufficient,
45, tab right through, boom, just copy what we did previously, 0.1, 45, we already know,
we don't care about that, we don't care about this, coming over here, now we'll keep this
at 2 inches, we'll keep the retract here, absolute all the way through, now the difference
here is, top of stock is zero, depth is zero, because we already put in our parameters here,
and this box right here dictates the cut, okay, so it's at a 45, so if it's 60 thousandths
off, it'll go 60 thousandths down, make sense? And it'll start from the line we selected
which was the inside, this looks perfect, let's go ahead and check it, boom, okay, now
one thing I'll say is, we're going to actually go to the inside and it's going to be an identical
path, so how about we actually treat it like that, I'll just hit this, I'll right click
here, copy, right click, paste, now we have an additional contour down here for chamfer,
now let's go into the geometry, boom, this box pops up, right click, re-chain, shift,
click on the outside, oh look at that, it looks so good, it looks so good, okay, so
now I say okay, boom, okay, boom, and there's another way to get it done, alright, and click
here, just say okay, and there's my tool path, alright, now if I actually want to watch it,
remember the S and B, S all the way through, B backing up, alright, now let's actually
zoom in, let's actually come in here, okay, okay, let's take a look, let's see, let's
see that, see that right there, it looks absolutely perfect, therefore we can look at it, have
extreme confidence that our tool path is perfect, I'll hit play, boom, speed it up a little
bit, beautiful, alright, check that guy, now as I stated before, I'm going to show you
a few different chamfer or deburr tool paths, right, so I'll go down, and then, oh, model
chamfer, now geometry, boom, I'm going to go on the inside line right here, and I'm
going to say, that's what I want, say okay, now avoid model, let's just put like 30,000
dimensions here, and what that's going to do, is it's going to make sure that your tool
stays off of this surface right here, okay, so you don't hit the part, alright, it's brilliant,
come back over here, boom, now because it's a different type of tool path, we have to
go ahead and reselect, so 4,000, let's go 25 inches per minute, nothing major, 100 inches
per minute, all of that looks good, cut parameters, we got 50,000 right here, that's perfect,
actually because it's a chamfer, let's actually use a bigger part of the tool, so let's sink
this a little bit more, so it goes off, and therefore I'm up here, which keeps the side
of the tool closer to the part, which allows this chamfer to get closer to the edge, okay,
so let's actually go 90, which is closer to half the diameter, which is 125, okay, so
90 plus 10, that gives you like 25,000 right here, just keeps you nice and tight, okay,
lead in and lead out, that looks good, that looks good, that looks good, I'm good with
all of that, boom, boom, multi passes, we don't care, clearance, we'll leave this at
zero, we'll keep this at 0.25, bead plane at 0.2, turn the coolant on, boom, hit this
guy and there you go, alright, so for those that didn't quite follow, let's actually walk
through it, okay, so I'm back plotting it, I'm going to play it, now I'm going to hit
S, I'm going to turn so we can take a look at it, boom, boom, boom, see how it's off
right there, meaning off in a good way, like it doesn't hit, hit B, hit S, it doesn't hit,
right, so that's the cool thing about that tool path right there, so we can go right
through it, boom, come out, okay it and now all of our chamfers on the top side are complete.
Now we're going to take the chamfer mill, we're going to chamfer these holes, we're
going to drill and tap and the part on operation 1 for the Titan 1M will be done. Alright,
so moving on, we're going to take that exact quarter inch chamfer mill and we're going
to spot these holes for our 10-32 tap, alright, so we're going to go to drill, boom, and now
we just need to show the software the positions of each hole, so I'll click this guy, this
guy, this guy, that guy, that guy, that guy and that guy and see I went from left to right
because I know my first part is going to be on the left side and then if I have a second
or third part, it'll be on the right side, therefore, the tool will start on the left
working its way to the right and then continue on down throughout the machine tool, so everything
looks good, I'm going to go ahead and hit this check, boom, I'm going to go to tool,
drill is already highlighted, so I'm going to go to tool, I'm going to click the same
tool, quarter inch chamfer, I'm going to double check, tool 3, tool 3, tool 3, 4000, feed
rate is 10 and I will leave that alone, alright, nice and gentle. Okay, so I'm going to go
over here, holder is fine, stock is fine, cutting parameters is fine, cutting parameters
is fine, everything is basically zeroed out and we're on drill and counter bore and I
am good with that, okay, so we'll drop down here, that looks good, that looks good and
now for linking, we're going to go ahead and hit our clearance, click this guy, it says
5 inches, let's just stay with 2 inches, retract height says 0.5, that's fine but let's just
go 0.25, again keeping this absolute, keeping this absolute, absolute, absolute, top of
stock is zero, that is correct, the depth of the hole, when looking at this thread,
I know that a 10-32 thread is about 0.190 to 0.192, if you want to be real, it's probably
0.192 diameter, alright, and roughly when dealing with a 10-32, the lead in or the chamfer
on the outside, we want it to be about 10% of the OD, outer diameter, okay, so if we
take 192 and we take 10% which is about 19 thousandths, we add the 19 to the 192, we
come up with 211 thousandths because it's a 45 degree tool, we divide that in half,
we come up with negative 0.1055, that looks good, come down here, coolant, turn the coolant
on, say okay and there you go, okay, so let's go up here, double check it, let's slow it
down, take a look, really close, let's just slow it way down and zoom in, let's take a
look at this guy, oh, look at that, it looks so perfect, alright, so I'm going to speed
it up, boom, boom, alright, so that looks great, I'm going to say okay, now our chamfer
is done and our holes are selected in perfect order, okay, so now all I have to do is actually
copy this guy for the next two tools, so the next two tools is a drill and a tap that's
going in the same holes, alright, so let's actually do that, so I'll come over here,
I'll right click, I'll say copy, I'll come down here, I'll right click again, I'll say
paste and then I'll do it one more time, there you go, so this is the chamfer, this
is tool 3, we're going to go in this guy right here, hit parameters, we're going to go to
tool, I'm going to go to .177 which is the drill size for the roll tap which we're doing
a form or roll tap and this is the hole size, okay, so I'm going to say tool 10, let's change
that guy, 4, boom, automatically changes, I'll keep this at 4000 RPMs, this guy right
here, I'll go 20 inches per minute, boom, that'll be fine, alright, that looks good,
we already know, I don't care about the holder right now, I don't care about the stock, the
cutting parameters, let's actually peck it, so we hit this guy right here on our pecks,
let's do a nice small peck, so we'll do 50 thousandths, boom, then I'm going to drop
down, drop down, drop down, so when we look at our prints for the Titan 1M, we can look
at sheet 2 of 3, down below you'll see that it calls out for 7 times the thread which
is a 1032 and it says a minimum depth of .380, so what I'm going to do is I'm going to send
my drill down 580 and then I'll send my tap down 480 which should give me the perfect
thread at 380, alright, taps don't have a huge lead so that should work out perfect,
so right now I'm going to say negative .580 and that's one of the key things, you have
to make sure that this drilled hole is deeper than the tap because when the tap goes down
it's not cutting material, it's pushing material and if it hits the bottom it's going to break,
so negative .580, now because I copied this, if we come to coolant, it should already be
on, so let's say okay, hit this guy, say okay and there you go, alright, now let's actually
go in, nice and deep, nice and deep, boom, boom, boom, boom, see, looks great, see that's
the cool thing, you know a lot of people say, hey you shouldn't teach programming before
somebody learns the CNC, but I believe once you're on the CAD CAM, once you design the
part and you know it intimately and then you program it, then the fear goes away because
you know that you have 5 tools, you're using a face mill, an end mill, a chamfer, a drill
and a tap and you watch the simulation and because you watch it, because you designed
the part, you know everything intimately, therefore when you go learn the CNC machine,
you know I just need to make sure that I duplicate the process in the machine, I hold the material
in a good solid vice and I set my offsets for my tools and my fixture perfectly and
you double check everything, then you're going to be solid, right, because you watch this
happen the entire time, okay, so I love that, boom, now let's just go to the next one and
you can see this is tool 4, let's go to the next one, hit parameters, now let's go to
the tool, oh we're almost done, this is good, so I'm going to go right handed tap, that
is our 1032, look down here, let's just go nice and slow, 500 RPMs, 500, spindle speed
15, it calculates perfect, alright, now I just noticed I didn't change my tool number,
so let's go ahead and do that, so it's tool 5, boom, boom, boom, perfect, alright, now
you can see it's tool 1, 2, 3, 4, 5, perfect, per our setup sheet, let's move on, boom,
boom, come over here, now up here, we're going to say rigid tap, boom, right there, see everything
is blocked out because it knows, it's going to go in and it's going to come out perfectly,
okay, now we just have to go down, go down and then double check our depth and over here,
we're just going to say the drill was 580, so this is going to be 480, okay, one thing
that I'll say is tool 5 on this setup sheet is a roll tap or a form tap, that pushes the
material and when it pushes the material, it retracts the material at the same time
creating the thread, now if you're using a cut tap, your ID or your diameter here is
going to be a little bit smaller, okay, and it's going to push a chip or pull a chip and
therefore your hole will have to be drilled in a way that allows for that chip to be pushed
in front of the tap, alright, that's just a little word, there's different types of
taps, so this is a roll tap and this will work out perfectly, okay, coolant is already
on, that looks perfect, I'm going to hit this guy, boom, go down, hit this guy right here,
say okay, now that looks good, I'm going to watch it, goes in, comes out, goes in, comes
out, speed it up, you know, when you're actually programming, you know, it's important to double
check everything, did I go 580 or 480, my advice is if you even double think it, if
you even consider that you might have made a mistake, simply click and go back and double
check, as a machinist, you got to always double check, alright, look how easy that was, I
went right back in, 480, yep, I'm good, super solid, and guess what, that brings us to the
end of the Titan 1M, I'm so excited, this is my first CAM, Mastercam program, it's the
first one, there's going to be more, we're going to tear it up, we're going to take you
guys to greatness, it's going to be amazing, Titans of CNC, teaching Mastercam.
Yeah, you guys have a great day, alright, boom.