Product Specialist Bhop Singh is back again to introduce a new feature that's available now on new Haas Lathes. That's right! We're talking about broaching keyways and other similar forms using Z-axis motion. Bhop shows us how our newly developed VPS Broaching template makes programming the motion easy and how G-code G156 keeps the code simple so you can make changes to your broaching operation easily.
Here is a link to our ST Turning Centers page: ttps://www.haascnc.com/machines/lathes/st.html
Normally when you want to broach a feature on a part you would need all this code.
This is about five pages long but on a Haas machine we've made it easy to turn those five pages
into one can cycle and you don't need to know how to program to pull it off.
My name is Bob Singh, I'm a product specialist here at Haas.
Today we'll be looking at how we use the VPS broaching template on this ST30Y.
Now early traditional broaching was performed on machines dedicated to that process alone
such as a shaving machine which used a shaped tooth that passed linearly against the surface
of a workpiece repeatedly to shear the material to the tube shape. Then came the use of push or
pull type linear broaching machines which use the same principle of shearing but use a long tool
with multiple teeth that gradually increase in size and depth to form the shape required.
Now I myself have run parts using both these broaching techniques many years ago and I found
that although they perform as required there are many downsides. Mainly fixturing, initial setup,
adjusting sizes and tool maintenance. In addition if you consider that a broach tool for a standard
3x keyway would stand over four feet tall you can probably imagine these don't come cheap.
On top of all that these machines and tools can take up valuable space on the machine shop floor.
In recent years the broaching process has been integrated into turning and milling operations
and although it's based on the same principles as the shaping machines from 100 years ago
the technical improvements in tooling and machines have greatly reduced the cycle time and costs.
The process to broach on a lathe is very basic. Orientate and lock the spindle at the location
required then using these broaching tools that come with interchangeable carbide inserts perform
the same movements as the shaping machine to form many different shapes on your workpiece. With just
basic insert and programming changes you can do keyways, slots, splines and even gear teeth.
Now here is a typical lathe program broaching using G90. Pages and pages of code that cut the
shape of a keyway. Each line on this program adjusts the x-axis ever so slightly in a positive
direction until it reaches full depth and if you need to increase or decrease the depth of cut
all this code would have to be rewritten. Haas not only created a VPS template to eliminate
programming for its customers but we also created a G156 CAN cycle specifically to condense this
routine to a few lines allow the user to make changes in seconds instead of minutes or even
hours. So let's set up this broach tool to machine some keyways into this bar. The material we are
broaching is steel and we are using a broach tool to form this 3x wide keyway. I will insert the
tool into the holder and indicate across the y-axis and x-axis to verify that the broach insert
is perpendicular and on center of the spindle. Now we'll use the probe arm to touch the tool
off exactly as I would do a boring bar. We will enter the VPS template by heading over to edit,
VPS and arrowing down to ID broach. The animation clearly shows that we're in the correct template
and our tool is in the correct position. Okay so I'll enter the tool number here,
the tool offset number and the work offset number we're going to use today is 54 for G54.
The next line asks what is the insert width. Our insert width for this part we're going to make
is 0.375 so I'll enter that here. The next line asks for what is the material we are cutting.
So we are cutting between a mild steel and an alloy steel so I'm going to enter M here. You will
notice as I enter different types of material, aluminum, mild steel and alloy steel that our
depth of cut starts changing and so does our feed rate. These are only recommendations and can be
changed by the operator at any time and I will change the depth of cut to one and a half now.
Next I will enter my bore size here. The next variable lets you choose the number of broaches
you want to machine. Default is set to single. We're going to change this to multiple broaches.
The broach start angle we will set at zero degrees and the number of broaches we're going to do is
three. This will machine three equally spaced broaches along the rotation of the bore.
The next line is asking for the keyway depth which is the T value and if you look at our
blueprint here we can see that it is 0.201 so I will enter that here. The next one is asking for how
far away from the face of the part do you want the broach tool to start broaching. We will choose
half an inch and the next line is asking if we want our coolant on or off. We would normally flood
the insert with coolant but for this video we will turn off that option so it's easier to see what's
happening in the cut. The next line we will enter the depth that we need to broach this part.
To achieve optimum results these inserts work best when they are centered and perpendicular
to the workpiece. They also like to exit the cut to a parallel face so if the back of your blank is
raw stock or not positioned true then the insert may chip much earlier than you'd planned for.
So if you are running this on a first operation with raw stock we suggest that you do what we're
doing here and that is move the broach operation to the second operation where the jaws are bored
and the blank exit face is parallel. If this is not an option then you could use a back face tool
or a groove tool to machine the back surface square before broaching and do not under any
circumstances broach all the way to a solid face. As robust as these inserts are they are designed
to push the chip forward and not evacuate them away so when broaching to a face on the OD or the
ID then a groove or cavity would need to be machined at the end of the broach keyway so the chips have
an exit point. The overall length of our blank is two inches long so we will go past that by a
hundred thou and enter 2.1 inches here. Now the VPS template is recommending 250 inches a minute
for our feed rate but we will change that to 400 inches per minute because the material we're using
has good machinability. Our final questions are just to retract the turret home
and how are we going to end the program. We will end it with an M30. Now I've entered all the
information into the VPS I'm going to press F4 and two we've got a program now let's run this.
As each pass reaches the end of the coat the I value in the G156 automatically retracts the tool
down a few thousands before it rapid back to the start position. This was created specifically to
help protect the critical sharp edges and corners from unnecessary wear when returning back in the
z-axis. And now the part's complete we can check it with our go and no go gauges to make sure the
is to spec. The gauge fits into the bar and the keyway smoothly and it is safe to remove this
completed part from the chuck. Here at Haas the VPS template and G156 code have made broaching
our keyways as easy as turning a diameter and if you turn this tool upside down you can now enter
our OD broach template to machine similar shapes around the diameter. You've got lots of options
for cutting these sorts of features on your lathe using G156 and our VPS template so if you've got
keyways and slots to cut definitely check them out. Thanks for watching and we'll see you next time.