How to tram a mill for best surface finish / flatness ?

dennh · Aug 25, 2008

When tramming a mill, what is a good compromise between surface finish and flatness? How much "tilt" per inch of cutter diameter do you leave behind?

It seems like it really depends on what your end goal is ... pretty finish or accurate surface.

johnoder · Aug 25, 2008

In over forty years I have never put it anywhere except as dead square to the table as I could get it. Otherwise the word "flat" is being misused.

John Oder

The real Leigh · Aug 26, 2008

I'm with John. Dead square.

Never heard of any other setting unless you want to get some kind of swirl pattern.

- Leigh

Commodus · Aug 26, 2008

dennh said:
When tramming a mill, what is a good compromise between surface finish and flatness? How much "tilt" per inch of cutter diameter do you leave behind?

It seems like it really depends on what your end goal is ... pretty finish or accurate surface.

I don't understand...why would tilting the cutter improve either?

machtool · Aug 26, 2008

I don't understand...why would tilting the cutter improve either?

For things like face mills or fly cutters. If you tilt the head ever so slightly, the tool doesn’t back cut or rub on the back side of the cut. One side it takes the depth of cut, when it spins 180 deg’s it’s just passing over the all ready cut surface.

Tilting the head actually generates a slightly concave surface, but the surface finish can look better, because the tool hasn’t rubbed. Depends if you going for accuracy or appearance. Works particularly well on aluminium.

Regards Phil.

Commodus · Aug 26, 2008

machtool said:
[/COLOR]

For things like face mills or fly cutters. If you tilt the head ever so slightly, the tool doesn’t back cut or rub on the back side of the cut. One side it takes the depth of cut, when it spins 180 deg’s it’s just passing over the all ready cut surface.

Tilting the head actually generates a slightly concave surface, but the surface finish can look better, because the tool hasn’t rubbed. Depends if you going for accuracy or appearance. Works particularly well on aluminium.

Regards Phil.

Oh I see...that makes sense. Though I admit, I'm having a hard time wrapping my head around purposely making something concave! Unless it's supposed to be of course...

Actually, I think that just provided a solution to something I might need to make at work! Yay!

Mud · Aug 26, 2008

I'm with Phil. It never seems to be exactly .00000 TIR, so I try to have it so that the leading edge of the face mill is lower than the trailing edge. .0005 or so over the full diameter of the cutter seems to be more than enough to eliminate swirl marks on a rigid machine.

Troup · Aug 26, 2008

Probably too obvious to need pointing out, but the more rigid the machine and cutter, and the less pushback force from the interaction of tool geometry (incl edge keen-ness) and material machinability, the less angle you need to eliminate dragging on the back cut.

machtool · Aug 26, 2008

I'm having a hard time wrapping my head around purposely making something concave!

The affect of the concavity depends on the diameter of the cutter. The larger the cutter the shallower the scallop will be. Its often used in production lines. I’ve set up a few OP10 & 20 head lines. They are normally where you skim top and bottom of the head. Normally that’s done with a really large slab cutter 16” or 20” diameter, even thou the head might only be 10” wide.

They were always canted over so they only cut on the leading edge, if you had them back cutting, and leaving a finish like this ()()()()()()(), that was another 16 or 20 inches of feed to get the cutter to fully pass over the head. That just kills cycle time. If they were canted so that only the leading edge was cutting, as soon as it passed over the head, it could retract and return.

I don’t recall a figure for how much, but it wasn’t a lot. I can recall guys, setting the back side with a cigarette paper, just so that it cleared the head. On such a large diameter, the affect of the scallop was negligible.

Regards Phil.

antique iron · Aug 26, 2008

Something that I do on my less than accurate old mills is to put 4 bolts in the T slots in a square. I mill these off all the same with a small end mill & then adjust the head to the tops of these bolts. This tunes the head to the travel of the table as opposed to the surface of the table.

Paul

gbent · Aug 26, 2008

For production work, I'm with machtool. Dragging the heel on a face mill will also wear out the carbide faster. On CNC mills where the spindle is dead nuts square I would feed out in Z during the cut. Somewhere between .0002 and .0005/inch would usually eliminate the backscratch. Only rarely could inspection find any concavity with the CMM, even when I told them it was there.

J Henricksen · Aug 26, 2008

On the big INgersolls, 8-12 inch face mill monsters, we would set the 'heel clearance' at .0001 per inch of cutter diameter. The only mills that didnt get that would be what was used to finish the ways on a mill bed.

Joe Miranda · Aug 26, 2008

As machtool and Gbent hav already noted it is the preferred method to have the leading edge of the tool slightly closer to the work piece. If you look at the Bridgeport manual for the alignment of the head, there is a note that reads,

"When indicating as in figure 3, it should be noted that the table is fitted to be slightly higher in the front, usually about .0005"."

The figure three that is referenced in the note is the tram in the "y" axis.

That being said, since I usually use my mill as a "jig bore" of sorts, I always try to tram the head as close to zero as I can so that all tools cut relative to each other as close as possible. This way when I switch from one boring tool to another I don't have to reindicate every time in order to hold positional tolerances.

Joe

Carl Darnell · Aug 26, 2008

I always tram/sweep the head in as near "0" with the indicator as far across the table as posible.

When using a flycutter the cut will lift the tool off the surface and on the back the spindle will drop down. The amount of back side cutting is dependant on the axial movement the bearings allow and as they wear it will increase.

If I am trying to get a flat clean finish I allow about .010" on the whole surface to go back and recut so I have minimal back cutting. Of course, with a worn mill it will still cut on the back side and some shops I worked in with well worn spindle bearings the back cut was guaranteed.

On the other hand, I worked in job shops and precision in the realm of .0001" was not looked for. We had a surface grinder and a Blanchard to do such jobs.

I do not think offsetting the head is a good idea because for normal mill work you are introducing an error unless you realign the head.

dennh · Aug 27, 2008

The reason for my original post was that I had trammed my BPT perfectly and was having a problem with surface finish in 6061 (home shop). I noticed that most parts received at work from a production CNC shop have a single sweep as if the cutter had a slight tilt. I think I'll take an indicator to some of them just to see what they're doing. It may be that they are doing what Gbent and others have mentioned.

Carl brings up a good point and that is the introduced error which varies with cutter diameter. If the error is within the allowable tolerance, I guess it may be ok in some cases.

Thanks for all the input !

Den

Carl Darnell · Aug 27, 2008

Den, I would think that the spindle bearings in a CNC mill have less movement than those in a BridgePort or knockoff copy. I am sure they do have to hold a better tolerance than a BridgePort.

madmachinst · Aug 27, 2008

If you use teh same mill for jig boring and edge milling and face milling. tram it "dead nuts on" you will just have to take lighter cuts when finishing. I usually plan my cuts for two finishing cuts and on hardened steel or aluminium ( any of the alloys). I get what looks like a ground surface. If you have more than one bridgeport so then certainly set one for finish cutting.

gentle · Aug 27, 2008

depends ...

Tramming a vertical mill is not really good practice. In my experiences, one would be sure that Y is perpendicular to the X table. This would be accomplished by mounting a granite square on the table and running the quill up & down along the square with a "tenths indicator. (a cylinder square is the second method) Lots of machines end up trapozoidal (sp??)instead of square with the tram method

Carl Darnell · Aug 27, 2008

gentle, what machine shop have you worked in that did that? That sounds like something a homeshop machinist that has all day to sweep the head in. I have never heard of anyone doing that. How would you ever be sure the surface plate is perfectly perpendicular to the mill table?

No, you don't use a surface plate or angle plate to sweep a mill head in, you use a dial indicator directly on the table or with a perfectly machined spacer, such as a bearing race, as some do.

Also, X and Y is the table moving side to side and front to rear and Z in the quill moving up and down.

LexD · Aug 27, 2008

gentle said:
Tramming a vertical mill is not really good practice.

Thats a hell of a statement to make.

How to tram a mill for best surface finish / flatness ?

Stainless

Diamond

Diamond

Aluminum

Diamond

Aluminum

Diamond

Titanium

Diamond

Cast Iron

Diamond

Stainless

Titanium

Titanium

Stainless

Titanium

Stainless

Aluminum

Titanium

Hot Rolled

Similar threads