Cut depths and spindal speeds to improve finsh time

Hi guys, at the moment I'm a moderately complex carving out of light density hard wood ( mainly American Walnut) 200 x 200 mm to a depth of 17 mm. To complete this its taking nearly twelve hours. I use a 6 mm end bit to rough out the block then a 3mm ball nose to finish. I have however realised that I could actually get away with a 6 mm ball nose that I will buy from flea bay tonight. What I was was wondering is , is there a cutter / bit that can cut at that depth in one go ? And what in you opinion is the maximum feed rate for this material ? Have you any tips for speeding up production please ? And one more question, I'm having trouble when swapping the bits from rough to finish as in they have different shank lengths and therefore I cannot simply push it to the top and it will be at the correct depth in the chuck, anyone any tips on how to swap out bits so they are at the same depth or should I just buy end and ball nose bits with same length shanks to make things simple ?

You may not be able to get same length shanks, and even if you do you will still need to reference them to the same length. If you make a collar to fit the shank and lock it off at your Z 0, you can then do the same to ensure your other tool has the identical protrusion. I use a length setting press and all of my tools always are exactly the same length. I have to admit it is easier for me as I only use 3.175mm shanks. G.

Id say you could do it on one go with a good carbide 6mm Ball 2 flute, you would have to ramp/zigzag down on the entry to the Max Z Depth at the start then travis back and forward using a mix of climb and conventional milling with a 0.2mm Step over. All depends on spindle and machine rigidity.

While it's possible I wouldn't cut 17mm in one pass has it will impact on finish and stress for tool, also risk of tearing the material depending on grain.
Quick Z level roughing won't take long with 6mm straight flute cutter and 3mm step which will greatly improve finish and work load for ball-nose finish cutter.

Regards tool change then your way of using shank length is asking for trouble and very unreliable. Bottoming the shank out in the spindle is bad for the spindle and it's bearings transferring heat and shock loads straight into it.

Presume because your not working off the material surface to reference new tool that you have chopped it away.? . . . In this case then you may find it easier to position your model in Cad so all moves will be in the positive direction and the bottom is at Zero in Z axis. This then means you can reference all tools off the bed and so long has you set enough rapid clearance height in Cam to clear material height you won't have a problem.

Another and far easier way if you use Mach is to setup a touch plate probe and use a screen set like Gerrys 2010. The CNC Woodworker - Mach3 2010

This has great feature for changing tools were after first initial touching off top of material it keeps track of the tool offsets and by touching off a fixed probe point it AUTO sets the tool height offsets for you and all you do is change the tool. Doesn't matter how far shank into spindle or tool length it does all the calcs and setting zero's etc.
You can even tell it where on the machine you want it to move too for changing the actual tool before it goes off and finds the new tool height.
If set up to do so it will start the spindle and carry on thru the code or wait for you to start spindle then carry on.

This combination of Fixed and moving probe plates means you can either very quickly manually set Z height off any point or like in this case were 3D model gets top surface cut away makes tool changes very easy and very accurate with the full Auto tool change.
Another Plus and great asset when used correctly and in conjunction with movable probe plate is the other probe options for things like finding centres of holes or circles, corners of parts, edges of parts, parallel edges etc

Thanks Jazz comprehensive as always mate :) I don’t think I have the skill to make a plate, but when I have the money I might ask someone to build one for me. I’m as usual over complicating things, maybe I’ll just get some 6 mm ball nose single flutes and do both clearance and finish with it ?

Quote:

---

Originally Posted by Fivetide

I don’t think I have the skill to make a plate,

---

No skill involved really and you won't believe how simple it is.!! Takes 10mins if that and in it's simplest form will cost no money. . . . I'll guide you thru it.

Just use a nice flat piece of aluminium or copper and fasten or solder piece of wire to it then take this wire to (+) of a spare input on your break out board. . . .That's it for the Plate.!!

If your machine has MDF or wood Bed then the plate won't need Isolating on one side but if your bed is Metal or ALi and you plan on cutting Metals then you'll need to Isolate the side that comes into contact with material, just use insulation tape.! ( Or instead of using Ali plate use Single sided PCB board)

Then go to Mach's Config/ports&pins/Input signals and set the Probe Input to the pin# used on BOB.

Now need to check plate is working correctly.? So go to "Diagnostics" tab and on the right you'll see lots of LED's where it says "Input signals current state".
The one called "Digitize" is the probe Input and it should be OFF. . . If it's on and the plate isn't touching ground or any metal part of the machine then go back into Ports&pins/Input signals and toggle Active Low setting. The Digitize LED should now be OFF.?
Now to check plate is working touch it to the tool and the Digitize LED should light up, touch it on/off few times to confirm. If it doesn't come on when you touch plate to tool then your spindle my be isolating the tool from Machine ground.? To get round this take another wire from ground (-) on the BOB and put a crocodile clip on end which you then clip to tool while Probing. Often this isn't needed and the tool grounds thru spindle ok.

Ok that gives you a working probe plate but now Mach needs telling what to do with it.?

This means we either have to assign some code to the "Auto tool Zero" button on the Standard screen set or use another screen set Like 2010.

I'll presume your using the Mach's standard 1024 screen set and will give code and instructions for that. This will only be the simple probe for setting Z height for when changing tools and will still require there be material left on top of part for the touch plate. (unless you work in the positive like I said in other post, then just put plate on bed.!)
If you want the more advanced setup where it uses a mixture of movable and fixed plates to set tool height offsets then you'll be better off buying Gerry's 2010 screen has it's getting more advanced and beyond explaining how to do in this thread.! . . . .I'd buy it anyway has it's other probes routines alone are worth it, not to mention much bigger tool-path screen.!

OK here goes.!!. . . . .First open the attached file and copy all the code in it. ( Where going to paste it some where else.!)

Then in Mach goto "OPERATOR" menu across top and choose "EDIT BUTTON SCRIPT". Now on the screen you'll see some flashing buttons, Click the "AUTO TOOL ZERO" button.
It will open the script editor and the page will be blank or have some simple message like this is empty.? Delete what's there and Paste the copied code into the editor.

Now this next bit is VERY VERY IMPORTANT !!!!! Else it won't work correctly.

Accurately Measure the Plate thickness. . . . Then in the code about 18 lines down you'll see line reading " PlateOffset = 0 ' Enter Plate thickness here "
Change this value to the measured plate thickness. If you don't do this then you'll get an error message saying "(Plate Thickness < 0 - Please Correct and try again)"

This has deliberately been set zero by me so you can't damage the machine by not entering the plate thickness. Normaly we have a place on the screen to enter this Value for ease of changing or using different plates which we then read in the script. This needs the changes to the screen set and obviously I can't do that without sending the whole screen set.
In reality you'll rarely change the plate thickness so it's no big deal and other than for ease of use it works just the same. If you want to change plate thickness then just change the script like above.

Below the " Plateoffset " is the Height the Z axis will retract after probing is finished " Zclear " you can change this value if you like.? I've set it to 20.0mm.
Again this would normally have it's own place on screen to enter and same applies.

When finished make sure to SAVE before closing editor.!!

That's it now you should have a working touch plate.

IMPORTANT !!!!! IMPORTANT !!!!!! IMPORTANT.!!!

Test the probe LED lights BEFORE YOU USE IT.!!
For the first TRY test it in the air not onto hard surface and keep your hand close to E-stop. Placing plate on a Sponge works well for testing and gives you time to hit E-stop if doesn't work.

Here's what happens.? . . . Probes in 2 stages: 1st probe is a fast initial probe at 250mm/min then retracts 3mm and probes again at 25mm/min it then retracts to 20mm above part and sets the Z axis DRO. . . . That's it now your Z axis height is set quick has that.:yahoo:

Now Disclaimer: Use completely at your own risk.!!
This code is a modified version of known good code and the same code I use and thousands of others but it has been changed for your needs and I've only tested it in simulation mode not on actual machine. Don't imagine you'll have any problems thou so don't be afraid.

If you have any problems let me know.!! . . . .Happy probing.:cower:

[QUOTE=JAZZCNC;42688]No skill involved really and you won't believe how simple it is.!! Takes 10mins if that and in it's simplest form will cost no money. . . . I'll guide you thru it.


Jazz is spot on, simple to make ( even I managed it! ), I use it all the time, makes using 2 or more bits on one job a doddle.

Fuck me ! Jazz thats awesome mate .. the only problem is I use NCstudio, as it came with the CNC and the board |:( But ill do some research see if I can replicate what you have said with it .. watch this space .. thanks again mate :)

Quote:

---

Originally Posted by Fivetide

Fuck me ! Jazz thats awesome mate .. the only problem is I use NCstudio, as it came with the CNC and the board |:( But ill do some research see if I can replicate what you have said with it .. watch this space .. thanks again mate :)

---

Ah I see no worries sure it will help others.? . . . . Anyway you'll want it later when you realise how shite NCstudio is and Ripout the NCcard for a PP BOB to use Mach. .:thumsup:

:hysterical: Priceless!

Quote:

---

Originally Posted by 2e0poz

:hysterical: Priceless!

---

What's tickled your Tit's.?

Tiz shit agreed.. next time I will know though lol ! And i'd like a bit of tit tickling plz !

It’s like that scene with the cancer patient in Flight film.. “Do I think god gave me cancer? No, do you think he would have given it me if I‘d have asked him to? No. Now I have it do you think he will take it away? No. Course I believe in God.. !!

As for a tool height setting probe, you could always make one like mine - http://www.mycncuk.com/forums/tool-t...-solution.html

(Yes, I am still alive..!)

Sorry Jazz i was reading the thread all serious how you was helping out then it was like someone popped your balloon. Can i buy you a new one to say sorry????

I will admit i am feeling guilty but it was funny......... I went into factors a couple of months ago to get some bits for my car. I asked for some parts for a nissan praire. The guy disappears for about ten minutes and returns with a shed load of bits. He says to me " i knew i had a bunch of stuff hanging around, you can have this lot for nothing as i will never sell it". I had to disappoint him and say i drive a nissan largo. He looked all puzzled to which i replied that if i had said they were for a largo he would not have known what the hell i was talking about. He was quite pissed that he wasted all that time digging the stuff out. I id get the bits i needed though.

Quote:

---

Originally Posted by 2e0poz

Sorry Jazz i was reading the thread all serious how you was helping out then it was like someone popped your balloon. Can i buy you a new one to say sorry???

---

No worries.!! It took 10mins from my day so no big deal and like I say sure others will benefit.
Must admit I didn't think to ask, mainly because thought I'd seen in another thread Fivetide used Mach.? Obviously mistaken Identity.!!

Quote:

---

Originally Posted by JAZZCNC

No worries.!! It took 10mins from my day so no big deal and like I say sure others will benefit.
Must admit I didn't think to ask, mainly because thought I'd seen in another thread Fivetide used Mach.? Obviously mistaken Identity.!!

---

I bought the board to convert it to Mach 3 then looked at the wireing diagram and though bolloxs to that this works so i'll use it .. and I still like tits strange really as my ex wife didnt have any.. go figure

Quote:

---

Originally Posted by Fivetide

I still like tits strange really as my ex wife didnt have any.. go figure

---

No Tit's is good enough grounds for divorce in my Book.!! . . . Having a Mach BOB and not using it is criminal thou.!!!

Get it swapped over man there's only 15 wires can't be that hard to figure out.! . . . . Will be worth the trouble just to use the probes. You'll also get better cut quality from what I've seen look here. Mach3 vs NC-studio

Quote:

---

Originally Posted by JAZZCNC

No Tit's is good enough grounds for divorce in my Book.!! . . . Having a Mach BOB and not using it is criminal thou.!!!

Get it swapped over man there's only 15 wires can't be that hard to figure out.! . . . . Will be worth the trouble just to use the probes. You'll also get better cut quality from what I've seen look here. Mach3 vs NC-studio

---

We are lol .. but now shes put on some wood and according to my Dad has a decent set of paps now ! NCstudio is shite ! but I need to live with at for the time being.. cash flow etc. Is sold the BOB coz I need the cash but one day I want 3 -4 machines running of the same board.. dream on lol
Oh and the good news with the new cutter I have halfed the cut time, and I also see ways of bringing that down by another 50% so from 12 hours to 2.. which is a bonus. Though my maths is shit its still 2hours

Well just in case people want the same for Linux cnc try this, works for me.

For Science » LinuxCnc

Im having the same problem only Im cutting 25mm mdf. 110mm alphabet A to Z. Im using a 6mm spiral Leitz tool. Spindle speed set at 5000rpm and feed at 7000 although I have this slowed down to 40% as strain on tooling . Im cutting this in 2 steps but its taking over 2 hrs to cut 144 letters..boss thinks Im swinging the lead. If I speed the rpm and feed up it breaks the tool. Are my speeds correct?

Hi, No expert, but I cut 15mm ply and 15mm mdf at 6m/min and 18k rpm using either straight or spiral 2 flute cutters and break very few. I am of course aware that I will probably be told that I'm doing it all wrong!!! G.

Quote:

---

Originally Posted by GEOFFREY

Hi, No expert, but I cut 15mm ply and 15mm mdf at 6m/min and 18k rpm using either straight or spiral 2 flute cutters and break very few. I am of course aware that I will probably be told that I'm doing it all wrong!!! G.

---

Not by me Geoffrey your cutting spot on IMO.

But what size cutter are you using?

Quote:

---

Originally Posted by deebo

But what size cutter are you using?

---

6mm cutters and forgot to add that I cut in a single pass.