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.

Similar Threads:

• open source cast iron box way benchtop milling machine
• Cast Iron
• cast iron machining
• cast iron question
• Cast iron milling problem

[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]

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

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]

.... 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]

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?

[Khalid]

Hi Geof,
The 4mm cut was done by the bit and it cut like butter... but I don't know why the Quill moves downward.. I think their is some PLAY(clearances) in the Quill that first adjusted and got a deep cut and for other passes those clearance cater for and showd no problem..

Currently I am making a new spindle and i will mount the Motor with Belt.. The whole system will goes up and down so no need of Quill.. I will show the results..


I just want to ask why you said the Machine is not designed/ rigid for cutting metal?
Regards

What about the above Oblonged Circle.. I think this was the Steps/Unit setting of the Y-motor and seems no backlash issues...This is because After each roughing pass the circle was remain same toward C/Y side( marked on the workpiece) but the cutting shifted toward the Top quadrant only...Any thought and ideas?

[Khalid]

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?

Welcom Wes

We have a Bolt to manually lock the QuillUpward/Downward movement.. The Quill has guide slot and the bolt is used to tight on the slot.. This help to hold the Quill tight.... but if i lock it my Stepper will unable to move it up/down...

Do you have any pictures of the JIG to limit the travel of Quill?... The Quill travel is 150mm (6 inches) and the Quill is guided through the body of the Head where we found 0.2mm clearance...

Do the quill has run-out adjustment? I don't know..

[Khalid]

Following is the description of above Cut... What is wrong?.. Is it backlash or step per unit?

[metalworkz]

Hello Khalid,
OK, so the stepper is moving the quill and the head is locked on the column. (I'm sorry, on my mill the Z head is moved with the stepper and the quill moves separately) If that is the case then there may be some backlash/play in the drive for the quill, right? I see where you posted above about making another spindle to use that will not use the quill for movement, and that sounds like it may help with the problem you are having.
I was thinking perhaps you could do the rough machining in sections so as to avoid Z movement and then you could use the quill lock and see if you still get the change in cutting depth and the out of round cuts in the circular pattern?
Then perhaps the minimal movements and cutting depth for the finish toolpath will not cause the quill to go deep and perhaps the adjustment could be snug on the lock to take up any play?
If you are going to be cutting more of these you will want to find a better way so maybe the spindle you mentioned will get you there, but it might be good to know for sure if the tightened quill improved the cutting of the part.
Regards,

[Khalid]

Hello Khalid,
OK, so the stepper is moving the quill and the head is locked on the column.

Yes, The Head is loccked on the round column and the stepper is moving the Quill.

(I'm sorry, on my mill the Z head is moved with the stepper and the quill moves separately) If that is the case then there may be some backlash/play in the drive for the quill, right? I see where you posted above about making another spindle to use that will not use the quill for movement, and that sounds like it may help with the problem you are having.

The Z-head is very heavy and i can't drive it with my stepper motor... See the attached picture... You are right , i have a play in the Quill , it is basically the clearance between the Head Guide bush and Quill that drive through it...

I was thinking perhaps you could do the rough machining in sections so as to avoid Z movement and then you could use the quill lock and see if you still get the change in cutting depth and the out of round cuts in the circular pattern?

I can't lock the quill... Actually I have locked it for the second rough pass and i forget to unscrew the bolt at the finish of rough pass... The lock was tight so stepper couldn't moved the Quill for second rough pass .. So I Feed stop the Mach3 and manually adjusted the Quill for second rough pass and i wrongly commanded in MDI screen to go up the Z-axes, and it instead goes down and you can see i have a Hole in the periphery of the Cut piece..

Locking the Quill is no solution for me because I have to do multi pass rough machining and 3D contouring...

If you are going to be cutting more of these you will want to find a better way so maybe the spindle you mentioned will get you there, but it might be good to know for sure if the tightened quill improved the cutting of the part.
Regards,

Yes locked Quill gave me smooth surface finish...

you can see the detailed pictures here
http://www.cnczone.com/forums/showthread.php?t=105247

[metalworkz]

Khalid,
In the graphic for the circular cuts do you know how that diagram is orientated on the machine axis? Is the 99.8mm side on the Y axis etc? Since the one side seems to stay at 99.8mm for each pass I would be tempted to think the problem is related to the axis of movement for the 102.7mm side? Can you check the axis calibration for that and perhaps calibrate it? I guess it could be a combination of backlash and steps calibration so perhaps look at one or both of those. I do feel the quill being lose allows the tool to wander also but I would think that would be seen around the circumference and not in just one direction.
Regards,

[Khalid]

Wes,
You are absolutly right.. I have to tune the motor 'Y-axis' that is giving me 102.7mm ..I will do it tomorrow and will make some circles and rectangles by attaching Pen to the Quill... Then I will see how close i calibrate the axis..

The X-axis (max-travel-300mm) and i calibrated it with 297mm gauge block and it gave me repeatability of 0.01mm throughout the length...

I have seen your work, what is the accuracy of your system? If you pocket a circle what tolerances you get after machining?
Regards

PS:
The X-axis side shows= 99.8mm
The Y-axis side shows = 102.7mm

I think on the X-axis side the 0.2mm is due to the Quill!!! Am i right

[metalworkz]

Hi Khalid,

I have an SX3 CNC mill from Syil and I made a small CNC router that I just finished not too long ago. My mill is very accurate but I did have a problem with a motor coupler on one axis(X axis I believe) being lose causing egg shaped or flats at 90º intervals of a circle. It has been good since cutting a flat and tightening the coupler.
My small CNC router is very accurate also, but the Rotozip motor run-out seems to be giving me some minor problems if I don't use very minimal pass depths on aluminum. I use a Craftsman type small router motor on my mill to cut wood and aluminum, but it does not seem to be as bad as the Rotozip for run-out.
I cut some precision aluminum parts on the mill and although I have never actually measured the accuracy I am able to hold .005" easily in aluminum to .50" thick and it is probably even better than that. I have tuned my CNC router to be very good with mach3, but have not done too much aluminum and most of the parts have been non-precision things like dog tags and axis labels etc. I do know I need to make a better spindle and that is in the planning stage along with a 5th axis B/C head.
Yes, maybe the quill is causing a slight run-out and it may be all along the circumference, but how will you know for sure without some sort of test?

Regards,