Facemill Hammering, solved

My original posting titled "Facemill & MT2" raised several questions. Andrew Johnston suggested that my width of cut was rather narrow. The hammering persisted, but it was lessened by following suggestions in that thread.

Now solved. Recently reading John Harvey's book "M/C Shop Trade Secrets", Harvey pointed out that using too large of a cutter (40mm in my case) relative to a narrow workpiece can cause hammering. And, his solution works a treat. You must position the cutter over the work so it is tangent to the work. The goal is to make the longest possible chip. My way to visualize this was to make a full size sketch of the work and position a clear circle over the work, aiming for cutting the longest possible chip. The solution is that the cutter will be tangent to length of the workpiece.

Of course, everyone knows that, but I thought I should post it just in case someone else might find it helpful. I appreciate the many helpful posts on this site.

Thank you.

Paul

Hi Paul thanks for letting everyone know that you have sorted your problem, to many times we don't get to know the outcome of the problem.

David

Hello Paul,

Harvey's book is a useful read, he has other helpful information gleaned from long usage that can save those treading the path a lot of back tracking as well as having useful tips, it is aimed more at Bridgeport use but the methodology is universal.

Regards

Brian

Not sure what you mean by "tangent" to the work. The path of the cutter is essentially a circle. The resulting work / cutting locus is generally a rectangular shape. Do you mean the cutter should be placed centrally and it should be smaller diameter than the workpiece, so that it makes a semicircular cut? That means a 100% engagement, which few people seem happy to do.

To avoid hammering you are going to want to ensure continuity of cutting ie try to get the second tooth to start cutting before the first tooth finishes its cut etc.

You'll never manage this with a flycutter or a single insert / single flute milling tool. Furthermore, unless you use a large fraction of the flute length on a fluted end mill, you won't achieve that on a multi flute cutter. It's always a good idea to use as much of the flute length as you can, otherwise you only wear out the tips. Reducing this hammering is another reason for doing so, although the advice is generally to avoid full width slotting and instead go for something like 20% stepover/ optimal load.

Murray

Muzzer: Thank you for your response and questions.

I, too had trouble with Harvey's meaning of "tangent", until I made a simple 2D pencil drawing and played with an imaginary (transparent circle) endmill hovering over the drawingl. Harvey's main suggestion is to make the cut-length as long as possible to avoid hammering. This took a few trials on paper to understand when that would and would not occur and why Harvey described this arrangement of the cutter's path as "tangent" to the workpiece. I had to lookup the Wikipedia definition of tangent and relate that to the imaginary "tool-path". If it helps, ignore the "tangent" concept and focus on "maximum cut-length". I think tangent is tangential to the solution.

As is so often the case, the cut width and depth were limited by the drawing/project conditions. So using the full length of the flute to "load and dampen" the tool was not possible. Also not possible to use the full cutter width. The task was also not a slotting cut, I think it is called a profiling cut (along the edge).

Yes, as you suggested, a second tooth in the cut would balance the load and reduce cutter deflection (which makes the hammering sensations worse). In the imaginary case, it can be seen that two of the four teeth were in the cut when the cut length was at its maximum.

The available tool was a 40mm carbide insert 4-flute facemill and the workpiece 20mm width. Why? Because this event occurred in a Vocational-Tech classroom with tooling limitations. Many of us must carry on with less than optimal kit.

You asked: "Do you mean the cutter should be placed centrally." No. If you place a 40mm cutter centrally on a 20mm wide workpiece, I found that the cut-length will be quite short (and per Harvey, you will truly get a hammering effect as the insert is then positioned nearer to 90° for much of the shortened cut-length. Harold Hall also explains this in his WPS: Milling, a Complete Course via Sk.4.

James Harvey's suggestion was to try to use a cutter not much wider than the workpiece (not practical in this case).

Paul

.

The oversize cutter is positioned not central to the workpiece, but such that it only skims one edge ... this provides the largest possible length of arc, and no interruption.

MichaelG.

Not only that (see M Gilligan above) but the 'tangent' method ensures that every cut is in the same direction, so any slack in the gibs etc will be pushed always the same way, rather than slamming from side to side.

If I understand correctly

- Cheers, Tim

Also, not really quite the same thing but obviously using a wide facing type cutter can put a larger load on the machine, as you're essentially increasing the width of the work it has to do.

So it's better to choose a relatively narrower cutter to remove more material first, when the finish isn't going to be a concern at that point, before then stepping up to the larger cutter for a thin skimming cut, tends to be less time consuming and tedious, than taking multiple passes with the large cutter. 

This doesn't become an apparent problem until you start trying to deal with iron castings and harder steels, i guess you can get away with it on plastics and certain aluminium. 

Michael W

Edited By Michael-w on 30/08/2018 20:43:42

Michael-W

Thank you for that additional comment re: cast iron hard spots, hardel steel and other alloys. In my original request, the 40mm insert face mill was knawing/hammering on a pre-hard alloy AXA toolholder. It was the only carbide cutter available at school. Our instructor was old-school and preferred HSS (as did I), but HSS.cutter could not cut the alloy.

Does anyone know more about this Tangent method? It was not covered elsewhere. And seems to.be essential aspect of milling in certain instances.

Paul

"Tangent Method", "Tangential Milling Technique"

I have since discovered that Harold Hall in his WPS Complete Milling Book talked about this method, but did not call it by this name.

He describes in a project reducing the height of a workpiece by profile milling along the X axis, then turning the corner and moving along the Y axis, turning again and continuing the cut along the X axis, then Y back to the origin. Some have called this a "chasing pattern". It saves time. It keeps the clearance forces of the gibs and v-ways going in the same direction and under certain conditions can accommodate climb milling. Andrew Johnston has (in another posting about milling) talked about keeping the cut "tangential" to the work.

I was talking about this with Ketan at ARC the other day and did a couple of sketches to illustrate the amount of contact time the insert on a 4 tip cutter would make run centrally down the work vs "tangentally" down the side. As you can see when run tangentally there is almost constant cutting, the only time you get a bit more knocking is at the start and end of the cut.

50mm cutter, 25mm stock centrally placed

Same tooling but work offset, one tip starts cutting as the other exits so bear constant engagement of the tool

JasonB:

This also makes it clear why it is important to reduce feed when entering and exiting a cut. Thank you for sharing.

Tim Stevens mentioned how the "Tangent Method" tends to maintain a positive force on the [gibs/table dovetails], thus reducing clearances/backlash. Someone called this a "chasing cut" and it works well when rough facing. This can be followed by parallel climb cuts for the finish if that is a cosmetic preference.

An open question (for me) is whether one can safely combine the "Tangent Method" with climb cutting. Is it risky to use a solid EndMill (EM), an insert EM or a FaceMill or does it depend on the material and/or axial depth of cut (ADOC)?

Andrew Johnston says he uses climb milling, mostly, but I have not been able to discern from his postings just when it is safe to do so. I've had my share of dodging HSS while experimenting.

Paul

It's safe when Andrew is using his CNC

A lot depends on the rigidity of the machine but most should be able to do light finishing cuts by climbing or if you want to save some handle turning a light cut can be taken when the cutter is returned before taking a heavier cut in the conventional direction. Nipping up the gib locking lever will help reduce the tendency for the tool to grab.

One problem with such cuts is if there is any appreciable slop in the splines driving the mill spindle.

My poor old Beaver mill has 9° of play on the six spline spindle drive. That works out as 15% of the total space is slop . It really bangs and hammers away when using a shell mill on a partial cut.

I've got the head apart at the moment and a replacement drive spline is one of the repair/rebuild tasks (the male spline on the quill has only got 0.002" of wear on 0.25" 'teeth', it's the female driving spline that's wrecked). I'm really hoping that this will help.

What sort of slop do other folks see on their spindles?