I am fairly knowledgeable with Haas mills (programmed VF-5 for 2 years making thrmoforming molds) but I have recently taken a job with a company that has 6 Haas lathes that I am not familiar with at all. Here is my task at hand: I have to machine an optically precise parabolic spline using a Haas SL20-APL (belt drive). We are trying to achieve a 4 to 6 micron finish off of the machine with no second operation polishing. My first question is am I asking too much of the machine we have purchased. This is a brand new machine (less than 6 months old and machine tolerances that should accomplish what I need). I have posted the code from Mastercam as both linear and arc movements with less than satisfactory results. When cutting the finish path of the spline I can feel what I consider to be excessive machine vibration. Question number two is when using high speed machining in this program (ie. G187 E.0005) it does not seem to improve the path. Am I using this application incorrectly? Should I be using diamond coated cutters? How much material (6061 or 7075 Alum) should I be removing on the final finish pass? I know for a fact that the optic I am trying to acheive has been duplicated in injection molded and stamped parts so there is know reason I should not be able to duplicate a machined part out of aluminum on a lathe. I have exhusated all of my ideas, any advice for a lathe rookie would be greatly appreciated.
I can not answer your question, but I have many questions.
What is the equation of your parabola, its size, and male or female? Is there a hole in the middle?
Have you used a very sharp tool, and what is the tool material?
What is tool nose radius? Have you tried making your own tool from high speed steel?
Do you get a difference between 6061 and 7075?
What feeds and speeds are you using? Can you change the finish by changing these? Finish depth of cut?
Is the finish better or worse at different radii?
Can you correlate the problem to spindle rotation, or to tool motion?
If you cut only one axis at a time X or Z can you get the surface finish you want? Is a facing cut worse than a longitudinal cut?
What are the incremental motions generated by Mastercam for linear or arc motions? Is the surface finish problem related to these increments, or is it uncorrelated? Is linear or arc interpolation better?
Is your program so large that you have to drip feed?
Is the vibration you feel carriage motion, or is it the belt drive spindle, or related to the spindle motor adjusting for constant surface feed?
Do you have to cut near zero radius, or is there a hole in the center of the parabola?
The following site post, by "rklopp" on "Finally some SHARP negative rake inserts" posted 2006-01-15 01:23, might be of some use
3. machine dependent motion control of X and Z axes, as distinguished from the effects of the program commands?
For example if you program a cone or arc is the surface finish poor within that one command vs the transitions from one command to the next.
4. 3 in combination with surface speed control?
5. does the transition from one command to the next cause a time delay in the X Z motion?
I have looked at a part that I machined a number of years ago, probably on our original HL1 rather than our current SL20. I do not know the parameters. The material was 7075 and probably used a Kennametal honed tool made for steel.
Visually the surface looks fairly good. This is 1.5" dia, then necks down via a 0.375" radius to a 0.75" dia, and then back up to 1.5" dia via another 0.375" radius. The straight 0.75" dia has better finish than the 0.375" arcs. Cutting pitch looks to be about 0.001" to 0.003"/rev. There are other modulations in the surface of a longer period, maybe 0.05" to 0.075". Surface roughness might be in the few 0.000,1" range.
This 0.05 to 0.075 period is more obvious on the arcs.
These are judgements more than actual measurements because one has to view the part at just the correct angle to see the effect.
First of all, Thank you for the detailed response. I will attempt to answer the questions you listed:
There is a hole in the center of the parabola approx .625 dia. The cut is a female cavity. There is a definite finish diference between the 6061 and 7075. The 7075 has a better surface quality just not good enough. We tried a near zero tool nose last night with no better result. Surface speed definitely changes the cut quality and we have experimented with a large range of speeds. Material removal on the finish pass is .002. I have not checked surface quality of a single axis cut with the same parameters but that is a great idea and I will try it out tomorrow. Unfortunately the shop is closed today. We do not have to drip feed the program, it fits in the control. There seems to be some harmonics going on that do not seem right to my, there is a definitely an unbalanced sound from the belt drive. But since I have never been around this machinery before I do not know if it is normal or not. Right now I am just trying to systematically eliminate all possible variables that are effecting the finish. Your help will definitely help me eliminate a couple of those things. Thanks again.
It may not be easy but if you have a high resolution electronic gage, probably meaning an LVDT, that you could resolve 5 to 10 millionths of an inch, then do a runout test on the spindle. There may be various periods to runout components.
Half revolution may relate to ovality of bearing components. Once per revolution to lack of squarenes or non-concentric components. Once per about 2.25 may be cage velocity. The cage is the element that spaces the balls or rollers. And then there is ball or roller component at less than one revolution.
In some respects a pattern on the surface can be used as an oscillogram and from this you might be able to find a relationship. So far we have been unsuccessful in finding the cause of a surface finish problem on a VF-3. But, you can view some photos relating to this at:
These photos are of no direct value relative to the lathe, but they give you an idea of the use of the pattern on the part as a troubleshooting oscillogram.
If you look at photos on our beta-a2.com site under the "MISCELLANEOUS PHOTOS page Relative to CNC" you can see some curved surfaces. But these are not near the surface quality you are looking for. The throttle body looks nice from a distance, but under a magnifing glass I easily see the cutting feed pitch. Thethrottle body was done on our SL-20.
You might try TapMagic for Aluminum instead of flood coolant.
In many respects we find our HAAS machines good to close to 0.000,1" in short path repeatibility. HAAS internally works with about 0.000,02" per encoder increment. A test I ran on our HAAS VF-3 with the surface finish problem showed 0.000,1" step increments to be within about 0.000,02" of their correct position over a back and forth motion of 0.000,8". This machine has zero backlash on the lead screws and we set the HAAS parameters for these to 0. The stepping measurement was measured with an LVDT resolving 0.000,005".
This is copied from your first post:
" I can feel what I consider to be excessive machine vibration. Question number two is when using high speed machining in this program (ie. G187 E.0005) it does not seem to improve the path. Am I using this application incorrectly?"
I looked up G187 and Setting 85 which it refers to and I wonder if it is possible you are using it the wrong way. This G code/Setting as I understand it is to prevent excessive corner rounding when your control has to perform an abrupt change in direction. There should be some sketches on the page in your manual explaining Setting 85 that show this. You have told the control to accept a small value for corner rounding so it will slow the feed approaching every corner. Actually the description for Setting 85 says if you enter zero the control will perform an exact stop at each motion block. Your program will have lots of motion blocks, each for a very small motion so with your small value you are forcing the control to slow and accelerate all the time very frequently; this could generate harmonic vibrations. You do not have any abrupt direction changes so maybe you could try using larger values for the G187 and see if this helps.