# How Should I Machine This?



## Metal (Aug 24, 2016)

Just a quick question really
apparently image didn't post, here
https://s10.postimg.org/hy9c8gjp5/dive.jpg




I'm still figuring out the new CNC, I've noticed that when coming around a corner, the bit has a tendency of being pulled up into the work exactly how I assume it would be due to the forces on the bit (note this is all roughing passes)

I "assume" this is unavoidable with a machine that has backlash since the mill moves upwards, then the torque from the cutter is what is dragging the table across the backlash zone and into the work before the cnc compensates.  if I was doing this manually I'd lock the table, which the cnc can't do.

So my questions  are
1: is this avoidable (I'm guessing not)
2: again assuming not, how much stock should I leave around the part for a finishing pass, My assumption again is around 2x the depth of the "dive" or .05", which ever is more, since passes less than .05" in aluminium tend to not cut it very well.


----------



## dlane (Aug 24, 2016)

I'll guess you are useing tapatalk camera icon , not paper clip , all I see is the infamous red "X"


----------



## jbolt (Aug 24, 2016)

What is the machine, material, cutter, depth of cut, width of cut, feed rate?


----------



## JimDawson (Aug 24, 2016)

I fixed the picture for you!

The first thing I notice from your picture is you are conventional cutting, if your machine will do it, climb cutting is the prefered method.

The next thing I notice is that your feed speed looks a little fast for the spindle speed. Maybe bump up the spindle speed or slow down the feed.  Your cutter could be a bit dull also, maybe try a different cutter.  Are you keeping the tool wet with coolant, I see what looks like fuzz ''welded'' to the surface.

Maybe try taking smaller bites, both depth and step over, it takes longer to make the part, but the quality generally goes up.  In the home hobby shop time is not normally an issue.  If you are doing this for profit, then some maintenance on your machine might be in order.  Maybe just snugging the gibs a bit would be helpful.

I normally leave 0.010 for the finish cut.


----------



## Metal (Aug 24, 2016)

Thanks for the advice, this was purposely roughing to test the cnc's accuracy at a higher load and with an old dull cutter since I wasn't sure if it was going to snap at this speed, I was just looking to address the dive issue circled at this time.

This is with a 3/8" endmill @ 1100 or so rpm, ~14ipm .1" doc.  6061 aluminium These servos could easily exceed 100ipm so I'm being gentle, I'm trying to resolve issues as I move up to a hopeful 20ipm cutting rate rather than just start at that rate and break a bunch of things figuring it out.

I am conventionally milling because the bridgeport doesn't have ball screws and its going to be less problematic.


----------



## Billh50 (Aug 24, 2016)

Jim is quite right in what he said. If your machine is not rigid enough you may want to take several passes conventional milling and leave about .015 for a final pass climb milling. Climb milling tends to leave a much better finish with the right speed and feed. But definitely use either a spray or flood coolant to keep chips from welding themselves to side as the cutter passes.


----------



## Metal (Aug 24, 2016)

so how would that address the dive issue illustrated above?


----------



## jbolt (Aug 24, 2016)

Your spindle speed is too slow for a 3/8" 2-flute cutter in aluminum for that feed rate. Would be okay for a 4-flute but with aluminum they don't evacuate chips well and tend to load up even running flood coolant.

I wouldn't recommend experimenting with a dull cutter. I don't think you will learn much other than dull cutters produce poor finishes.

I suspect the over run issue is the backlash on the lead screws. Are your gibs snug?


----------



## JimDawson (Aug 24, 2016)

Metal said:


> so how would that address the dive issue illustrated above?



Using a dull cutter will increase the dive.  The cutting pressures are much greater and much more spring in everything.  The cutter is doing more rubbing than cutting, especially when conventional cutting.  

Here is a staged picture of a bearing mount I machined last night just to put things in perspective.  Material is 6061-T6



I still had the G code loaded so I fired up the machine and grabbed a screen capture of the running machine cutting air.

The DOC is 0.125, a sharp solid carbide 3/8 end mill, climb cutting.  Kerosene in the fogless coolant system.  Finishing passes were at 0.010

This is real time cutting parameters.  The inputs come from the G code, actual spindle speed, and actual axis vector speed.  The cutting speed and chip load are calculated from the inputs.  Also accepts manual inputs for calculating feeds and speeds when not running.




This may help a bit getting you started in the right direction to address the issues.
.
.


----------



## Boswell (Aug 24, 2016)

I'm not sure I understand your initial post. Are you implying that you have 0.05 backlash?  If that is the case, you probably need to figure that out before making parts. No amount of optimizing feeds and speeds or coolant will fix a 0.05" backlash.   I also tend to leave 0.015" for a finnish pass and use climb milling most of the time.  For a 0.375 two flute cutter. 0.1 DOC at 1100RPM and full cutter width slotting, GWizard sayd that a very aggressive rough cut would be 7.9 IPM and (as a hobbyist with more time than money) I never use the most aggressive end and for roughing using go about midway between aggressive and conservative, in this case GWizard recommends 4.8 IPM .  I typically cut using 2750 RPM and in this case that would allow the 4.8ipm to increase to 12.3 ipm.  Also note that GWizard assumes you have proper chip removal in place (Flood coolant, or Misting system etc).


----------



## Metal (Aug 25, 2016)

adjusting gibs, stepping up the rpm a tad (48 to 50 hrtz on vfd) and reducing lead in speed seems to have helped (and adding the finishing pass), the features are slightly trapezoidal so I have backlash over compensating or leadscrew wear to address but I think we're okay at that point.

I was under the impression you don't want to climb cut in a machine with leadscrews unless taking very small cuts (or I could adjust the gibs /really/ tight(?)  so what is the story there?


----------



## TomS (Aug 25, 2016)

I climb mill on my RF-30 all the time but with a bit of caution.  I adjust the depth and width of cut to minimize the chance the cutter will grab and pull the work piece into the cutter.  My gibs are not adjusted tight but not loose either.  

I use climb milling almost exclusively on my CNC mill leaving about .010" for the finish pass.

Tom S.


----------



## JimDawson (Aug 25, 2016)

Metal said:


> I was under the impression you don't want to climb cut in a machine with leadscrews unless taking very small cuts (or I could adjust the gibs /really/ tight(?) so what is the story there?



It is related to backlash, when climb cutting the work is being pulled toward the cutter.  The heavier the cut the harder it is being pulled.  The machine has to be rigid enough to overcome this force.  If there is backlash the table can move uncontrolled for the distance of the backlash on a transition, this can cause the tool to grab.  Tightening the gibs will help by adding friction to the system, but you can only go so far with this.  The way to really fix the problem is to eliminate the backlash.

Does your machine have acme lead screws or ball screws?


----------



## Metal (Aug 25, 2016)

It has lead screws which is why I was sticking to conventional


----------



## JimDawson (Aug 25, 2016)

In that case, maybe the best bet is to do the roughing conventional, then climb cut the finishing pass(es)  Or just take smaller bites so the mass of the machine helps to overcome the tendency of the tool to grab.  Lighten up the DOC and stepover rather than reducing the feed.  The cutter needs to cut rather than rub, sharp cutters will help.

For any really serious work the only solution is to install ball screws, preferably double ball nut so they can be preloaded.  Unfortunately it's impossible to have a zero lash acme screw / nut.  If there was zero clearance it wouldn't turn.

I wish I had a better answer for you.


----------



## Metal (Aug 25, 2016)

I've had a backlash laden mini mill cnc'd for about a year, it hasn't been a huge issue for me, the bridgeport cnc is just proving much harder to tune up to where I want it.


----------



## JimDawson (Aug 25, 2016)

One totally crazy idea comes to mind, you could preload your lead screws with air springs.  Connect air cylinders to the X & Y axis on the table and it would eliminate the backlash.  I'm doing this with my Z axis, but I never thought of trying it on the table.  Probably not really practical.


----------



## Metal (Aug 25, 2016)

Well that certainly is one way of increasing resistance!

I could push the machine more softly, but truth be told I just don't want to run the bridgeport at full speed (over 3k rpm) until I get it tuned in, and have a shield of some sort in place since this is quite a bit scarier than my little hobby mill.  But I've picked up a handful cheap of 3 flute hss 12mm endmills that I'm not afraid of breaking that I'm going to try tonight probably with some new code to be a little more gentle once I properly setup backlash comp again.

I also need to rebuild the head as low gear is noisy and I'm getting grey oil at the base of the spindle probably because of it but that is for another day.


----------



## jbolt (Aug 25, 2016)

For projects that require a lot of material to be removed I've become a big fan of using roughing end mills for removing most of the material and only using standard end mills for finish cuts. Smaller chips, deeper cuts and faster feed rates.


----------



## JimDawson (Aug 25, 2016)

Metal said:


> this is quite a bit scarier than my little hobby mill.



I had the same problem when I first got my CNC.  Was scared to death of all that new fangled stuff.  I used it for about a year as a manual machine with a fancy DRO before I had the guts to actually run it as a CNC.  It just takes some time to work up to that.    It's a learning curve.  Now after about 3 or so years I have confidence in me and the machine


----------



## Metal (Aug 25, 2016)

Absolutely, in getting it working I had one servo runaway with the belts attached, magmotors at full spin are terrifying fast, I was luckily able to estop before the axis hit its endstop but in my mind that could have cracked the cast iron and I"d have a 3000lb paperweight in my basement.

I'm putting /huge/ rubber bumpers at the ends of travel due to being paranoid, but this thing is /awesome/ compared to the hobby mill, even at the above "conservative" 15ipm / .1 doc / less than half cutter engagement I can make the run for that part in the first post in under 5 minutes, that was like a 20 minute job before, plus fixtures/indicating because I could never get a big enough vice in the little one, and I'm not even going /fast/ yet.
It is pretty exciting that I am this close to getting it running, I'm close to a year in on this project, hah.


----------



## Metal (Aug 29, 2016)

I've got this tuned out now, I went to a larger, sharp, 3 flute cutter which seems to have removed the dive

Did some experimentation climb cutting, and even with a 1/4" ballnose not cutting much at all it wanders a little, so i'll stick to only using it for the final finishing pass. but moving on to more complex cuts and all is going well!
I'm having some minor accuracy issues with some parts, but I believe that is leadscrew wear which I can't correct for until I get good home switches.


----------



## JimDawson (Aug 29, 2016)

Sounds like you are on the right track.    That is a complex part, looking good!

I'm not sure how home switches will help compensate for lead screw wear.  Can you explain what you have in mind?


----------



## Metal (Aug 30, 2016)

JimDawson said:


> Sounds like you are on the right track.    That is a complex part, looking good!
> 
> I'm not sure how home switches will help compensate for lead screw wear.  Can you explain what you have in mind?



In mach3 you can create a grid basically, pick a spot on the table, tell it to move 1", then measure how far it actually moved in order to measure the wear on your leadscrew/nuts, off the top of my head I don't remember what the menu was (screw mapping?), but once you create the measurements mach3 can compensate for them so your parts dont end up slightly squished or stretched.

But anyways, in order to map out that grid and have mach3 know its relative position according to it, you need a home position for mach3 to reference.  Right now I don't have a home position at all so it has no idea where it actually is on the table, just from its work home reference point.

Ive also noticed that I get a "moan" from the right side of the y axis at a certain point in its travel, only when moving in one direction... which I need to figure out.


----------



## JimDawson (Aug 30, 2016)

Ahhhh.... That makes sense.  I remember seeing that screen.



Metal said:


> Ive also noticed that I get a "moan" from the right side of the y axis at a certain point in its travel, only when moving in one direction... which I need to figure out.



Strange.  It is possessed?


----------



## TomS (Aug 30, 2016)

I may be wrong but I thought I read where Mach3 has a limitation on backlash compensation.  In other words if your backlash exceeds the maximum allowable then BL compensation doesn't work at all or Mach ignores the incremental backlash that exceeds the maximum allowable.

Tom S.


----------



## JimDawson (Aug 30, 2016)

Do a Google search for 'mach3 backlash compensation'.  A lot of info on it.

I see double nut ball screws in your future


----------



## Metal (Aug 30, 2016)

I dont think its haunted, I think its the ways binding or some stuff got into them or wear on the ways (but they still had scrape marks so that would be strange), weird that its only in one direction.  

Backlash compensation is /fine/ I have it setup and it works great, the only issues I ran into was I had a mm indicator and imperial screws so I ended up with too many significant figures doing the conversion and ended up having to round it for mach3 to work right.

What i'm (vaguely" seeing is my parts end up being a few thou longer than they should be, even if only traveling in one direction, its not really a big deal for the kind of stuff I make, but I should probably fix it.


----------



## Metal (Aug 30, 2016)

May have figured out the noises, adjusting the gib appeared to do nothing, but adjusting the y axis belt did, it appears the servo belt drive is putting too much downards strain on the leadscrew or somesuch, i'll see if i can order a belt with one more tooth


----------



## JimDawson (Aug 30, 2016)

Cool!  One little step at a time, but you're getting there   One of these days some pictures of your machine would be a good thing.


----------



## Metal (Aug 31, 2016)

Sure, I've attached some of the cnc modifications.
I'm pretty sure the lube system doesn't work very well, but it is what it is.


----------



## JimDawson (Aug 31, 2016)

Nice installation!    Is that a NEMA 42 motor on the Z?  It looks huge!  How are you counterbalancing the quill to compensate for the backlash in the rack & pinion?

Some lube is better than none.  More is better


----------



## Metal (Aug 31, 2016)

Thats easy, I don't, since I only cut conventional and down ramping I don't seem to need to (or haven't run into it yet!), I do leave the plunge brake partially down to give it a little more resistance, but otherwise nothing special.  My plan was, in the distant future is it appears that I can slave axis's together in mach3, I could run a breakout board output to a relay of some sort, to a solenoid and have a little pneumatic cylinder engage/disengage the axis lock whenever that axis isn't moving, but that may be over complicating things.

Thats way after tuning it in, turns out that a scribe in a 1/8" collet is pretty concentric but I cant edgefind with it to save my life, or something else is still off, the tuning continues


----------



## Metal (Aug 31, 2016)

Also the part for today, 3 half done wheel frames for the robot, when I did the other side, again things got trapezoidal so I'll hit the meters again tonight and make sure I have that backlash set right, if not its got to be a zeroing or leadscrew wear issue.


----------



## JimDawson (Aug 31, 2016)

Here is a picture of my quill lock and the counterbalance cable connected to the quill stop.  The other end of the counterbalance cable is connected to a 1.5 inch air cylinder.  With the quill counterbalance, the Z will consistently hold 0.0001 (one tenth).  I have not implemented the quill lock yet. I have all of the parts, but haven't been in a big hurry to get it finished.


----------



## Metal (Aug 31, 2016)

You mean an air spring, not an air cylinder(?) if not when/how do you pressurize it, to what?


----------



## JimDawson (Aug 31, 2016)

Yes, air spring, I kinda misspoke there.    It is 1.562, double acting,  air cylinder, with air plumbed to the rod end, with a filter on the back end.  The airline from the regulator is T'd to about a 3 gallon air tank to keep a large air reservoir so the pressure stays constant, rather than relying on the regulator alone.  I run it about 35 PSI or more if needed for larger endmills.  The 2 inch square tube housing in front of the cylinder is where the cable to cylinder connection is made.  The assembly is attached to the top of the Z axis drive gear case.  The cable is about half of a Yamaha Banshee brake cable.


----------



## Metal (Sep 6, 2016)

Oh neat, thanks for the info.
I blew a gecko320x over the weekend so no machining for me for a while


----------



## JimDawson (Sep 6, 2016)

That sucks 

Oh BTW, I keep the quill counterbalance pressurized all the time.  At about 35 PSI it has about 50 lbs of up force.  Hardly noticeable when operating manually, just makes a nice quill return.


----------



## Metal (Sep 6, 2016)

Yeah I have no idea what caused it, I'm running 2 motors off of a 72v 20a power supply so it shouldn't have even been able to output enough power to burn up the controller, and it did it to the Y axis, while it was stationary and the X axis was slowly coming in to touch my finger (testing out a probe)  I've already shot gecko an email for repair/advice on what caused this and ordered a replacement (should have a spare anyway) 

Also found out my one shot lube system isn't delivering lube to all the points properly, ugh its always something isn't it
does that replace your clock spring(?)  I'm also noticing a hole in your head which leads to what I assume is the gearhead.  shouldn't that whole compartment be more or less full of oil?


----------



## JimDawson (Sep 6, 2016)

Metal said:


> does that replace your clock spring(?)



The clock spring is still in there.  The clock spring preloads the the Z axis drive gears.  The counterbalance actually preloads the quill rack & pinion.  This is how I eliminated all of the backlash in the Z axis system.

Depending on the Z axis drive system, you could eliminate the clock spring.  On a conventional lead screw drive you would not need the counterbalance or the clock spring.  I chose a gear system so it would be a quick changeover to manual operation, all I have to do is flip a lever and turn off the Z drive power.



Metal said:


> I'm also noticing a hole in your head which leads to what I assume is the gearhead. shouldn't that whole compartment be more or less full of oil?



There is very little oil in the head.  The back gears are greased and are above that area.  That hole is where the original quill feed engage lever was.  The only oil in there is for the external quill oiling, but not the spindle bearings.  It's the same area the the oiler on the right rear accesses.  Only requires a few drops per day and just drips out the bottom of the quill housing.

My head is pretty much gutted.  All of the quill power feed hardware has been removed.  The only original parts in there is for the the back gear and the quill pinion shaft.


----------



## Metal (Sep 19, 2016)

So making progress this weekend.
Added 20a fuses between the controllers and power supply and between the controllers and motors, everything should be good now, maybe

1.  Slowing down to 6-8 ipm climb cutting and doing a .04" finishing pass gives things a really good finish, I'm wondering if slowing down the feed overall and just going deeper to get roughly the same clear per minute may be the way to go
2.  Servo's overheating, I've rigged up some PC CPU fans to the x/y and will wire them up today, it takes about 30-45 minutes or so for them to get hot enough to concern me (still not too hot to touch maybe I'm overly concerned) so I figured with that slow of a warm up it isn't that big of a deal,  I was looking around, but couldn't find any heatsinks, I could have sworn that someone sold heatsinks where the base plate was thin enough you could just bend it around the motor, may have to make something.
3. I still keep losing zero, typically stop the cycle with the yellow button in mach3 which completes the current move then stops, turn off the spindle/cnc, leave it for 30 minutes or so, then come back and repeat the steps in reverse, I'm losing zero somewhere in here, and sometimes during tool changes.


----------



## JimDawson (Sep 19, 2016)

Metal said:


> 1. Slowing down to 6-8 ipm climb cutting and doing a .04" finishing pass gives things a really good finish, I'm wondering if slowing down the feed overall and just going deeper to get roughly the same clear per minute may be the way to go



Give it a try, a lot of machine work is experimenting to see what works best.



Metal said:


> 2. Servo's overheating, I've rigged up some PC CPU fans to the x/y and will wire them up today, it takes about 30-45 minutes or so for them to get hot enough to concern me (still not too hot to touch maybe I'm overly concerned) so I figured with that slow of a warm up it isn't that big of a deal



A 40°C temperature rise is common for motors.  If you can touch them, it's normally OK.  I have had steppers go to 145° F running unloaded, this is normal.  



Metal said:


> 3. I still keep losing zero, typically stop the cycle with the yellow button in mach3 which completes the current move then stops, turn off the spindle/cnc, leave it for 30 minutes or so, then come back and repeat the steps in reverse, I'm losing zero somewhere in here, and sometimes during tool changes.



What happens if you leave the CNC powered up?  How much error are you getting?


----------



## Metal (Sep 20, 2016)

I threw some pc fans on the servo's with zipties, and they are now ice cold after 30+m  before I had about 45m before they were pretty hot, so I think we're okay there.

I'm not sure yet how far it is off, but I'm resolving it for now by just taking a final finishing cut which should take up the .0x" that its off.
I've also discovered that my inches are about .001 too long, so some more tuning is necessary.

I'm getting a slight rattle in what sounds like the drawbar at higher speeds now too, hrm


----------



## bfd (Oct 8, 2016)

I would need to see your work (just like high school math) but itlooks like you are trying to climb mill instead if conventional mill. climb milling sets the cutter to climb up on the part and if there is any lead screw slop it will pull the part forward and cause it to dig in.climb milling should be limited to the finish cut for alum. .005" cut. reroute your direction of cut to feed the endmill so the cutting action is from inside the part to outside the part instead from over the top of the part. bill


----------

