how much wall stock do you leave in dynamic?

[lowcountrycamo]

Machine is a new Okuma mu4000 5axis table table.  We are machining ti 6al-4v.  I would like to leave .005 - .01 for 2 finish passes.   Stepping down between .5 and 1.2.  The less I leave,  the less the walls will flex on finish.   I just don't know how accurate the dynamic motion is.  On filter parameter page the total tol. is .001 / cut tol. is .0005 /  line arc tol. is .0005.  Create arcs in xy is checked.  Does this mean that the dynamic motion will hold true to .001 of model?  What exactly does the cut tol. and line-arc tol. mean?  Not real sure how the filter tolerances work.

Thanks,

Steve A

[Leon82]

I leave .005 with a .0025 tolerance usually with good results. I think I use 50% cut/arc tolerance It will over cut if your tolerance is bigger than stock to leave.

The machine is also running the aicc or the matsuura ips so it is not going to overshoot

[huskermcdoogle]

It is mostly the machine, not necessarily the path that determines this.  If you run in supernurbs or Hicut, you shouldn't have much overshoot, especially if you aren't running 500-1000 IPM.  I am guessing you are 250 IPM or less?  If so, shouldn't be much orvershoot or corner clipping going on at all, probably less than a thou.  So keep your tolerances somewhat tight, and don't filter at all and run point to point only in supernurbs, or filter, and don't let the path violate the finished part.

[nickbe10]

It depends also on the tool size you are following with (part geometry and size are also a considerations). With .5 inch and above (and all insert cutters) I generally leave .02 for finish for 2 reasons:

Ti is "tough", it does not want to start a chip. Leaving more stock gives the tool more to bite into. It might look like you are making chips but you might be "skipping" flutes which will lead to premature tool wear due to the skipped flutes rubbing not cutting (and generating heat).

Ti is also "heat resistant" so in order to prevent thermal distortion a larger chip volume helps in loading more heat into the chip and not into the part.

If I have an especially tall and thin wall I will generally rough and finish in Z level steps using a finish cutter with a healthy corner radius to help blend the steps.

If you have a very"3D" part which has a lot of steps after roughing then the steps can help you in starting your chip (more to bite, the stock left is the minimum between the steps)

With smaller cutters you can probably get away with less, but I never go below .01 unless I have a cutter less than about .093 diameter and I have made a one pass .01 finish cut with a .062 and nailed the nominal all day, speeds and feeds to balance the tool loads are key here.

Also if you leave .02 stock it allows you to make your base filter setting .002 (rule of thumb 10% of stock thickness). This can dramatically shrink your toolpath size and allow more arcs to "fit'.

[jeff]

I usually leave .005 or .010" per side depending on the material, how fast I'm running it, and the finish requirements.

[gms1]

I haven't had the opportunity to cut ti but everything I do cut I do like to leave some stock like nickbe10 does. I do believe I get better tool life and finishes when I leave .01" to .02"

[nickbe10]

4 minutes ago, gms1 said:

I haven't had the opportunity to cut ti but everything I do cut I do like to leave some stock like nickbe10 does. I do believe I get better tool life and finishes when I leave .01" to .02"

I started out leaving .02 stock when I was doing a lot of fairly large Ti hogouts (put the material on the machine with a forklift, take it off with a couple of fingers kinda size) on the advice of a Stellram Applications manager, he maintained that if you got down to 0.01 stock in Ti you were in serious trouble). It occurred to me that what was true for Ti was also true for Al as they have similar molecular structures, similar properties (the most important being heat resistance) and very similar tool geometries, so I went with the same there.

The result was more dimensionally stable parts and longer tool life just as gms 1 says, and as I outlined there are good thermodynamic reasons why this works.....

Of course if you are making small parts you can get away with lower stock but it will still lead to less tool life....

[gms1]

Yeah I guess I should add that I do not do anything small here. The majority of my programs are made for parts over 60" in length and I measure cycle times in days. So small widgets may lend itself better to leaving less stock.

[Leon82]

Our print will sometimes call out how much to leave for heat treat. 

Some invar prints say no cuts more .01 after heat treat

[nickbe10]

1 hour ago, Leon82 said:

Our print will sometimes call out how much to leave for heat treat. 

Some invar prints say no cuts more .01 after heat treat

A good point. I would be very wary of using insert cutters to make this cut reliably in Ti. Solid carbide, which has a sharper edge, if at all possible. Having said that I have been forced into a position where the solution I found was to use Aluminum grade inserts for light finish cuts. The corners went off pretty quick, but then things settled down and I was able to hold dimensional tolerance and finish (a really amazing finish actually) for enough parts to make it economic, I didn't need the corner rad for the cut. If you machine a lot of Ti, be prepared to "get out of the boat".

Most of these call outs are due to the thermodynamic characteristics of the material, again mainly its heat resistance. Because of these characteristics you do have to be careful when in process heat treating is involved. Thankfully most aerospace structural parts (where my experience lies) don't require intermediate heat treating. we just get the material in at the correct hardness, machine, paint and ship.....

There are also a whole bunch of restrictions (again in aerospace specs) on other processes such as deburr and non - traditional material removal processes like plasma cutting which many shops are unaware of.