| | |
We have some custom crankshafts to make and wanting to consider setting up our lathe to do the grinding of the bearing surfaces. At this time, we plan to purchase ground bar stock for the con rod journal pins so we would only need to grind the ends for the outside bearings. This is a pretty basic twin cylinder crank.
I was curious if anyone has done grinding in a CNC lathe? The guys we have talked to for grinding our parts said they could hold about +/-.0002". I figured we could hold that with a lathe if we do it right. Am I dreaming here?
Also, I would like to learn where we could get more info on bearing clearances and such. We will of course have to select the bearings before we will know what we have to hold for shaft OD tolerance.
Too bad we lost NC Cams!!!!
Bearing shaft and housing dimensions are available in the tech/engineering sections of most bearing manufacturers catalogs. Most are on line. Try "googling" SKF, BARDEN/FAG, NSK, NTN, TIMKIN, TORRINGTON ETC.
Are you referring to the front, center and rear main bearing positions when you say "ends"?
Dick Z
DZASTR
This is a motorcycle type crank but there are radial ball bearings at each end and one in the center dividing the two crank halves.
BIG loss with NC Cams. I was trying to find him today when I discovered the news. Guy taught me a LOT!
( The guys we have talked to for grinding our parts said they could hold about +/-.0002". I figured we could hold that with a lathe if we do it right. Am I dreaming here ?)
Your not dreaming,we used to grind od bearing surfaces on rear end housings and easly held +/- .0003 and that was on modified engine lathe.
As far as on a cnc that could be interesting,(a few more variables then doing it manually).I sort of remember a post asking a question like this before,maybe a check through past posts may dig something up.
Just push the button,what's the worst that could happen.
It was probably me to be honest. We have had several jobs that we have pushed away over the years because we could not afford to outside grind the parts though they really did need grinded (part callout tolerance was just tighter than we felt we could hold and were bearing surfaces). Honestly, just trying iy could prove a good solution.
What kind of extra "challenges" are you referring to? I really do not feel the programming or dressing will present a challenge, just the tolerancing, wheel selection, feeds/speeds, etc are what worry me. NOT experienced with grinding so I have no clue but I planned to just program passes with say a .0002 step over with a pretty fast feed and WFO on the spindle speeds to keep the surface speed up.
(What kind of extra "challenges" are you referring to?)
Well not a challenge so much,but I can't say how it would work on cnc.When I did it,it was manual so it was about the feel of the handle and the look of the sparks ( good days they were). I would just look into doing it on cnc a bit before going ahead with it. A few questions might be with dressing the wheel and then grinding the part,how to find size again,beside checking and adjust?
(I think in doing many parts not just a few) so could I trust if I dressed .005 of the wheel to take that much off the offset for doing the part ???
If I pretty much know the outcome I'm ball's to the wall,but when I don't, well slow and steady wins the race.
Just push the button,what's the worst that could happen.
Grinding Bearings Hello, I am new to CNC zone. This is my first post. I used to work as a department lead grinder at a bearing plant. I ground raceways, od's Id's etc. if you could attach a ridgid spindle to your cnc center, it could be done. One thing worries me though. when grinding od's, generally the wheel is usually much larger than a 2 inch or 3 inch part. This is to eliminate "chatter" / waviness eventhough you could stretch any situation. you could definately grind internal surfaces with the cnc being your machine is in good shape; considering, I am talking aerospace results. I know all the speeds and feeds if you need them. good luck. you also would definately need a wheel dressing system if you are in production.
Its like this. grinding about 60 thousandths of mild steel stock, you need to dress the wheel about 4 to 5 times total. You cut .015 then dress--cut.015 then dress--cut .015 dress--then cut .013 then final dress--come back in and grind the last .002 and dwell on the part for 10 seconds. use an iscolating motion back and forth-each end of the wheels face surface reaching the center of the part. NOTE: different material (harder/softer) uses slightly different tecniques
anything is possible, I am worried about the finish.
Last edited by engineerstudent; 06-04-2009 at 04:41 AM. Reason: add something
I moved this one to the machining forum (from engineering), hope you get even more answers.
Yeah, NC was the perfect person to answer questions like this.Originally Posted by viper6383
From personal experience, I would use .0006" +.0003"/-0 In excess of .001 would be too much IMO
Too much shink-fit and your bearings will over-heat and the bearing life will be reduced. Not enough shrink fit, if the bearing spins, you can imagine.
And from personal experience, zero your bore gauge using your micrometers and double check the dimensions of the bearings your using.
MC
I would hate to subject a typical cnc lathe to wheel dust (primarily from dressing the wheel) and have it circulate around with the coolant.
Grinding wheels can induce their own form of waviness to the journals that they grind, if the wheel has any eccentric runout. Sometime it is very difficult to eliminate all runout, even dressing a vibrating wheel does not always fix it. I've seen this many times just after pulling a bearing off a journal (on an electric motor). It is virtually undectable to the indicator, but your eye can see it easy. And that type of mass production grinding is done, I assume, by guys in the grinding business with wheels that they treat with TLC to attempt to get the best results.
I do precision turning and boring with the lathe and the mill, just so I don't have to put up with the mess of grinding. What kind of lathe have you got that cannot hold .0002" from part to part? Yes, I might have to work at it, and inspect frequently to adjust tool offsets, but that only takes seconds, and it is easily understood the effects of the adjustments, without introducing a whole new gamut of headaches, such as learning the finer techniques of grinding.
Generally, I hand finish journals (in small production quantities like 50 to 100 pieces) by polishing on a speed lathe. A perfect amount to remove with polishing is about .0002", as this comes off quickly and then you are down to the basic diameter that will 'stay' over repeated removal and reinstallation of bearing races. Also minimal polishing ensures that the journal stays cylindrical (as turned) and not tapered. It takes some technique to polish straight cylinders, and not have the ends oversize or rounded off.
If quantities are high, then probably getting a real grinding machine would be a better long run option, or farm that aspect of the work out.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Posting Permissions
| | |
LinkBack URL
About LinkBacks
