Need Help!- Milling Cast Iron

[Khalid]

I have recently converted Radial drill Machine into 3-axes CNC, and now experimenting with milling a simple impeller of Diameter 165mm and Height 40mm...
You can see the retrofit here (2-pages only), for judging whether this machine can do Steel milling or not!!!!!
http://www.cnczone.com/forums/showthread.php?t=105247


The stock i intend to use is Cast Iron. The EndMill for rough cutting has diameter of 10mm HSCo, 2-flutes Brand New DORMER. following are the feed and speed i calculated:


Cut Feed: 7 IPM
Spindle speed: 727RPM
Cut Direction: Mixed i.e. (Climb+Conventional Mill)
Depth per Pass: 1mm
Step Over: 25% Tool diameter
Engage/Retract: Helix
Toolpath: Horizontal Roughing
CAM Software: VisualMill 6

Unfortunatly,I have broken one of the end mIll when after 3rd Pass it plunged into the material and cut 7mm deep and 1inch length and i stopped the machine.. I read the toolpath and i found nothing strange... The Tool was broken from shank and one of the flute was chiped-away near the tip.

I have 0.1mm runout at the tip of the tool... kindly help me how can i reduce the machining time and how can i avoid breaking the tool...

Your help at this moment is highly appreciable.. so don't skip please answer me with your experience.

Regards

Can someone guide me, what better i can do?

PS:
kindly note that this is my first time milling Ferrous/non-ferrous material, so help me please.

[advt001]

Did the endmill pull out of the holder?

[Khalid]

No , The tool remaining shank was tight in the collet... I further investigated on Z-axis Quill drive, but there is no way that the quill drive itself..This is because the Quill is driven by Worm-wheel mechanism and back-drive is not possible......

I was getting vibration during each plunge moves so i reduced the DOC to 1mm included the Helical entry for each plunge and this solved the vibration problem...

Tomorrow I will try with all of your help again.. Today i was much disappointed..

I am thinking of PLUNGE ROUGHING technique...

Regards

Any help will be appreciable, and ask many questions i will give you all the details...

[Geof]

For machining cast iron the tools should have zero top rake. Milling cutters with a helix always have some effective top rake because of the angle of the helix so it is best to use a cutter with the lowest angle available. It is also better to use four flute cutters for a more even cutting load. Your cutter very likely pulled down in the collet because the helix angle acts likes screw, particularly a high helix angle, also with a 25% step over one flute has left contact with the work before the other makes contact so there is a pulsating action on the cutter which can accentuate the pulling out.

Try using a four flute cutter, drop the speed to about 500 rpm, take a deeper cut something like 3 or 4mm and drop the feed to 5ipm or even a bit less. Also if possible use a setscrew type holder and a cutter with a flat on the shank for the set screw to locate on (Weldon shank I think it is called). This will prevent the cutter pulling out.

Incidentally what type of cast iron is it. Malleable, ductile or nodular cast iron machine best. Gray cast iron is not as good and the hard skin can cause problems. White cast is really difficult to machine.

[Khalid]

Hmmm.. Just thinking after carving with 150IPM on wood for 5-years, How bad i am feeling when i crawl with 7IPM on machine and i am getting in the simulation software the rough machining time 40Hr for this small part

For wood it would only take 1.5Hrs complete...

[Geof]

Machining cast iron is slow, very slow compared to wood. The trick for machining something from solid is to rough away as much as possible with a large diameter cutter than move to a smaller cutter for finishing. This means you need a good sturdy machine with a decent amount of horsepower so you may be out of luck.

[Khalid]

Originally Posted by Geof For machining cast iron the tools should have zero top rake. Milling cutters with a helix always have some effective top rake because of the angle of the helix so it is best to use a cutter with the lowest angle available. It is also better to use four flute cutters for a more even cutting load. Your cutter very likely pulled down in the collet because the helix angle acts likes screw, particularly a high helix angle, also with a 25% step over one flute has left contact with the work before the other makes contact so there is a pulsating action on the cutter which can accentuate the pulling out..

Hi, Geof You are The Man of Knowlege and Wisdom Thanks for answering and guidance...

My cutter was not pulled down in the collet, but it plunged into the workpiece and the high torque X/Y motor then took it apart just below the collet.. Half of the shank inside the collet in tight position where as the remaining tool was in the workpiece.. Unfortunatly i don't have pictures right now...

I agree with you about the helix angle.. Also i have a runout of 0.15mm on the tooltip (I can't reduce it Any idea?)..I will try to find the right tool

Originally Posted by Geof Try using a four flute cutter, drop the speed to about 500 rpm, take a deeper cut something like 3 or 4mm and drop the feed to 5ipm or even a bit less. Also if possible use a setscrew type holder and a cutter with a flat on the shank for the set screw to locate on (Weldon shank I think it is called). This will prevent the cutter pulling out. Incidentally what type of cast iron is it. Malleable, ductile or nodular cast iron machine best. Gray cast iron is not as good and the hard skin can cause problems. White cast is really difficult to machine.

You are genious.. Sure I will reduce the RPM and take the deep cut with very low IPM say 2~3 IPM... Hmmm.. the cast iron is locally casted and really i don't know the composition or type.. How can i recognise those types?...

I have to make the same impeller with 15-4PH steel.. and in future i have to machine Stainless steel on this machine.. I don't know will i able to work with it or not... if You have seen the pictures of the machine (link posted above)you can tell me whether it is possible for it to work with SS316?

Thanks for answering

[Geof]

Originally Posted by Khalid .... Hmmm.. the cast iron is locally casted and really i don't know the composition or type.. How can i recognise those types?... I have to make the same impeller with 15-4PH steel.. and in future i have to machine Stainless steel on this machine.. I don't know will i able to work with it or not... if You have seen the pictures of the machine (link posted above)you can tell me whether it is possible for it to work with SS316? Thanks for answering

It is probably what is called gray cast iron which is used 'as cast'. Ductile, malleable and nodular are heat treated following casting.


Can you work with 316 on your machine? Difficult to give an answer. 316 work hardens under the cutter so you need to be able to take a depth of cut greater than 2mm or so, and a feed per tooth of 0.01 to 0.02mm depending on the size of the cutter. If your machine is not very rigid you are best using HSS or cobalt tools, not carbide, so this means you have to keep the speed down to around 100 fpm to be conservative; so you can only do things slowly.

[Khalid]

Originally Posted by Geof It is probably what is called gray cast iron which is used 'as cast'. Ductile, malleable and nodular are heat treated following casting. Can you work with 316 on your machine? Difficult to give an answer. 316 work hardens under the cutter so you need to be able to take a depth of cut greater than 2mm or so, and a feed per tooth of 0.01 to 0.02mm depending on the size of the cutter. If your machine is not very rigid you are best using HSS or cobalt tools, not carbide, so this means you have to keep the speed down to around 100 fpm to be conservative; so you can only do things slowly.

Hi, Geof
Today i have machined a Pocket 100mm diameter upto 4mm depth.. Two rough cuts with 1.5mm and One Finish cut 1mm...RPM were kept the same 800RPM and the Feed was 2.8IPM..
I have some issues with the Quill.. Initially the tool ramp into material and start spiral cutting... after 20mm diameter tools went down about 0.1mm and i ended with about 3mm deep with step upto final machining...

The region between 30mm and 100mm was flat with 3mm depth of cut for the first Rough machinging (It should be 1.5mm deep but i got 3mm deep with steps i mentioned)... The next roughing operation start at the same location and the cut was 0.5mm deep and it levelled the whole Pocket... then exact 1mm down cut was done with finish machining...

My Gcode was perfect but i think the initial down of the cutter upto 3mm deep shows me some serious problem with quill or backlashes in gearing mechanism at higher vertical load... How can i compensate???

I also found the circle a little oblong toward North-South direction about (1mm) but i not found any backlash issues as the cutter start and end at the same locations and i didn\t got any step marks... May be I have to check and calibrate the steps/unit of X-axis motor..

I have side clearance of about 0.2mm in the Quill...and when the tool engage it goes back 0.2mm i think.. So


In the circle i got

102.7
-
-
------ ----- 99.8
-
-

[Khalid]

Attached are the pictures....
The C-Y marking side= 99.8mm
and the other quadrant the dial shows:102.7

The variable depth at the periphery was due to i stopped the machine and manually raised the Z-height for shallow cut at the end of final finishing operation...


PS:
Attached is the pic of broken tool 10mm HSCO , 02-Flute

[Geof]

It sounds like your machine is not rigid enough for cutting metal. I am not experienced in tuning steppers or servos or trying to figure out backlash compensation so you have gone past the point I can be of any help.

[metalworkz]

It sounds like the quill is not locked, does it have a means to lock the quill movement? Perhaps you can fabricate a jig to limit the quill travel so it cannot be moved during cutting? Also does the quill have any provision to adjust the runnout at the quill?