Often times CNC programming tutorials only teach you how to create the tool-paths and not enough attention is paid on showing how to properly hold parts being machined.

At the same time efficient workholding is an art in it self and mastering it could drastically improve shop productivity and accuracy.

Without further ado let's jump into the workflow.

Step 1. Analyze the Drawing and the Model

We would have to look at the drawing, tolerances and the CAD model to develop the machining strategy.

This particular part has tight (+/- 0.001) tolerances between the features located on the top and the bottom sides. In addition to that it has a 2.5 degree draft angle on external walls.

Thus I decided to not use the soft jaws approach and machine it in a fixture. Soft jaws are generally OK for tolerances down to +/-0.001" but because of the draft angle the part would always want to pop out of the jaws.

1. Finished Part 2. First Op: Before 2. First Op. After 3. Machined Fixture 4. Second Op: Bearing Seat 5. Third Op: Finished Part

One of the most versatile ways of clamping irregular -shaped parts is with use of soft jaws.

In this one I had to machine a triangular-shaped part from two sides.

It is going to be some sort of a part holding jaw for a robot.

So step one: Machine one side of the part in vise. hold on to 1/8" of stock. So make sure to cut your part on a bandsaw oversize.

Step Two: Bolt soft jaws to your vise and machine a pocket using outside contour of your part.

Be sure to relieve corners.

Step three: Clamp your part in the soft jaws and machine the second side of your part.

One important thing to consider is: this method is not very accurate. depending on the size and a shape of your part you may be able to hold it within 0.001" though.

See attached photos of the steps below.

1. Machine one side 2. Machine pocket in soft jaws 3. Clamp the part 4. Machine the second side

Recently I had to machine a few pieces after turning.

Because the very top of the part was supposed to be machined off, I could not clamp through the central hole like I often do.

Decided to quickly turn an expandable washer out of aluminum and a plastic spacer that would collapse a little bit under clamping pressure and allow the part to sit firmly against the base of the fixture.

I liked this method so much I am going to do the same next time I have similar part to make.

See pics below.

Later on i will try to post some more pictures of other setups I did.

All the pieces apart Fixture, spacer, expandable washer, FH screw Workpiece mounted on

HSM or High Speed Machining is becoming more and more popular each day.
Many of us have seen those youtube videos where endmlls remove large amounts of material at high speeds/feeds.

While definitions of HSM may vary between tool manufacturers and even individual shops, the physics behind it remain the same.

In this article i would like to explore flat endmills.

HSM is not about ramping up your speed/feed overrides to 200% and puling out your smartphone to record another youtube-worth video.

What is HSM?

HSM is a complex of programming, machining and tooling techniques aimed at radical increase of productivity.

Programming

The cornerstone of HSM is low radial and high axial engagement of an endmill with the workpiece.

There are many CAD/CAM systems that allow you to create HSM tool-paths. Mastercam's Dynamic milling and SurfCAM's Truemill are some of them.

When radial cutter engagement with the material is smaller than the radius of the tool an interesting thing happens.
Chip load- the distance the tool advances per cutter revolution per tooth- does not equal the actual chip thickness anymore.
Chip thinning mainly happens at radial engagements below 30% of the diameter.

In order to get compensated chipload you need to multiply recommended by manufacturer chipload by the chip thinning factor.

Usual Radial Engagement for HSM toolpaths however is between 5 and 15%.

Axial depth of cut varies depending on geometry, but

Radial Chip Thinning HSMAdvisor Screenshot

I recently had to machine an aluminum mold cavity.

7 inches deep. With 5 degree wall draft and a 60 thou radius going all the way down. Roughing was not an issue, but for semi-finishing and finishing i had to manufacture these two extension holders.

Both tools have runout of less than 0.001

The one for bigger 3/8 tapered ballnose cutter is shrink fit- i mounted it using torch.

The smaller tool is a 3/32 tapered ballnose cutter from Harvey Tool.
I could not bore to correct size, and had to ream right on.
The tool is mounted with a set-screw from both sides to prevent deflection caused by unequal clamping pressure.

13640634846051.jpg

Anybody could use a pair (or more) of push clamps around their shop.

Those handy devices convert your machine' table into a huge vise.
They are pretty mush irreplaceable when machining plates and other oversized parts that no ordinary vise will fit.

Several vendors offer their clamps. But many of them tend to be pricey. And those that are not, lack in quality.

And to be honest with you, it does not look like they are worth the amount of money their seller is trying to get from you.

In the mean time their design is simple enough to fabricate in any shop.

Here is a picture of two of four clamps i made for myself on manual mill withing 2 hours- sure beats buying mitee-bitees for 175$ a pop!!!

Made out of 5/8" thick D2 plate

1" long Shoulder in the front is tapped to 3/8-16 NC.

Slot for 1/2-13 bolt is sloped towards the back to prevent clamp from sliding under clamping pressure.

A thick 1/4" washer is used to protect T-slot from damage by the socket head.

I ll try to get more pictures tomorrow.

IMAG0540.jpg Drawing

Hi-helix end mills have several advantages inherited with their design.

Simple math says that a an endmill with 45 degree helix angle directs 50% of the cutting force downward versus  25% for a 30 degree end mill.

Main advantages are:

• Higher rake angle directs more of a cutting force downward.
  This reduces side load on the cutter, that leads to less deflection and less tendency to chatter.
• At high axial engagement (deeper depths of cuts) more flutes remain in the contact with the work piece. This leads to much smoother cut, again reducing tendency of the cutter to chatter.
• High helix angle pulls chips upward and away from the cutting zone.
  This reduces chip re-cutting and helps prevent cutter from getting clogged up. This also allows to take deeper cuts and increases productivity.
• Because of higher helix more of flute length is being used in the cut. Better surface finish is achieved even when using the same chip load.
  Generally an end mill with 45 degree helix can be fed 30% faster than equivalent one with 30 degree helix and still achieve same surface finish.

High helix end mills also have disadvantages that a machinist has to take into consideration:

• With more of cutting force directed axially, the load on spindle bearings in downward direction is increased.
• Tendency for both the end mill and the work piece to pull out is increased. So a more rigid tool holding and work clamping should be considered.
• Higher helix end mills are also less stiff that regular helix end mills. This may cause more deflection and may become a problem when having to machine straight walls.
  This effect should be mostly diminished by lower side radial load, but it still needs to be considered in some cases.