I need help regarding basic milling

More
04 Dec 2021 09:41 - 04 Dec 2021 11:06 #228336 by PhilipME
I am trying to understand the basics of milling while trying to put my DIY milling machine into use.

I used the following
feed rate : 90 mm/minute
tool : 4mm end cut/ 4 flutes/carbide
stepdown : 0.1 mm

things going very well with no vibration please see the short video


My question : I have the metal shavings welded to the edge of the cut . Is it because I am not using cooling water? and running at high 5000 rpm. I do not see any indication of excessive temperature. I can touch the plate near the working area not hot at all. For sure the tool maybe very hot.

Second question : how do I remove the chips every few minutes? if I press the pause button on the axis interface screen and raise the tool up along z axis and clean the chips, and then hit resume button on the axis interface screen is this the proper way to do it?

Many thanks

Note :

1-this is not the spindle I intend to use. just for experimenting. Also I will place order for cooling mist nozzle.  I am only investigating the potential of the DIY machine to be or not to be.
2- The other holes in the plate you see are made by laser machine.



Philip


 
Last edit: 04 Dec 2021 11:06 by PhilipME.

Please Log in or Create an account to join the conversation.

More
04 Dec 2021 11:38 #228342 by piasdom
first. your rpm is too fast for metal. you're rubbing the metal not cutting.i'm surprised the plate is not hot. try 1500rpm and YES use coolant. even if you just squirt water on it. you can use a brush to remove shavings without stopping machine. hope this helps
The following user(s) said Thank You: PhilipME

Please Log in or Create an account to join the conversation.

More
04 Dec 2021 12:11 #228343 by PhilipME

first. your rpm is too fast for metal. you're rubbing the metal not cutting.i'm surprised the plate is not hot. try 1500rpm and YES use coolant. even if you just squirt water on it. you can use a brush to remove shavings without stopping machine. hope this helps



 

Defenetly it helps

thanks

Philip

Please Log in or Create an account to join the conversation.

More
05 Dec 2021 02:25 #228374 by spumco
Phillip,

You need to not 'guess' at the cutting parameters.  I suggest getting machining software (some is free, some is low-cost), or looking for a web site which will help you set the starting feeds and speeds.

I'm assuming you're very new at this so I'll explain feeds & speeds:

Speed - this is the surface speed of the cutting tool where it contact the work to be cut.  In the case of your mill, the tool diameter and spindle RPM will determine the surface speed.  Usually expressed in feet per minute (Imperial) or meters/min (Metrique ;). Also known as "SFM" (surface feet per minute).  The surface speed is completely dependent on the tool material, tool coating, and work material - regardless of cutter diameter or tooth count.

Tool manufacturers publish a range of surface speeds appropriate for a given tool & workpiece material.  Uncoated carbide in mild steel should be run around 45-120 M/min (based on a number of published sources).

Feedrate - this is the speed the tool advances through the workpiece. It is usually expressed in inches or mm/minute.

Chipload - If you don't want to guess at the feedrate, then the typical way to calculate the appropriate feed rate is to determine how thick a chip is to be taken per tool flute.  Usually expressed as inches per tooth (IPT) or mm/t.  If using chip thickness, the feedrate is a derivative calculation made using the desired chip thickness (feet per tooth), times the number of flutes, times the tool RPM.

Using your example:
(your cutting data)
RPM - 5000
Tool Dia - 4mm
Feedrate - 90mm/m

Result:
Surface speed - 62 M/m
Feed per tooth - 0.004mm per tooth.

The 62 M/m surface speed is perfectly appropriate for carbide tool in mild steel.  However, the feed per tooth (and consequently the feedrate) is not remotely in the ballpark.

Your cut was essentially burnishing or rubbing the tool and not actually cutting much.  This dulls the tool, heats it up, heats up the part, and - as you saw - can weld the chips/dust to the part and tool.

I tend to use a minimum feed per tooth of 0.001" (.025mm) with carbide in steel, unless the tool is extremely fragile. Less than that and the tool can rub and get damaged.

There are a million web sites with explanations about starting parameters for milling/machining.  Go find a site and try out some of the suggested feeds & speeds.  You can always go slower and lighter if the cutter is deflecting or chattering, but don't take too light a cut per tooth.  Slow the RPM down first before slowing the feedrate.

-Ralph
The following user(s) said Thank You: tommylight, PhilipME

Please Log in or Create an account to join the conversation.

More
05 Dec 2021 09:35 #228378 by PhilipME
Thank you Ralph

I realy appreciate you taking the time to provide this very useful input.

The issue being that I do not want to spend the money to retrofit the machine for the bt-30 spindle if the the machine will eventualy turn out to be incapable of milling steel.

So the only option I have is to experement with this G-Penny spindle .

Knowing that the spindle will be at risk at lower RPM, and the spindle bearings were not designed to handle severe shocks generated between the tool and the steel plate, so that is why I am in this situation.

After I found that I could not penetrate the plate (At that time I did not know why), I made the tool approach the steel plate from the edge (Very dump)

The reason I did that is to force the system to generate vibration even if I end up breaking the tool. So I got what I wished for and broke the tool.But I learned what I wanted to learn and that is the rigidity and stifness of the frame will be capable to proceed with the retrofit with the bt30. At least this what the situation looks like unless I missed something.

I have a very cleart path-forward now, but I have so many wood related projects for the machine. So I will wait for the retrofit when I finish the wood related projects.

your post in this thread and previous threads where valuable and where implemented or taken into consideration.

Thanks everyone

Philip

Please Log in or Create an account to join the conversation.

More
05 Dec 2021 16:08 #228389 by Michael
Also it looks like you are machining A36 structural steel. Very common steel type. A36 however is not very friendly to machining. It is very gummy and inconsistent. You can machine it but I would toss my end mill afterwards.

As a replacement source 1018 steel to get the same strength but free machining characteristics. I can usually cut 1018 at close to the same speeds and feeds as aluminum in my small machine. Mostly because my machine can't go fast enough in aluminum.
The following user(s) said Thank You: PhilipME

Please Log in or Create an account to join the conversation.

More
06 Dec 2021 01:02 #228411 by PhilipME

Also it looks like you are machining A36 structural steel. Very common steel type. A36 however is not very friendly to machining. It is very gummy and inconsistent. You can machine it but I would toss my end mill afterwards.

As a replacement source 1018 steel to get the same strength but free machining characteristics. I can usually cut 1018 at close to the same speeds and feeds as aluminum in my small machine. Mostly because my machine can't go fast enough in aluminum.




At this learning stage with so many variables, and with a new DIY machine that run for the first time, the last thing I want is to take the harder route.


I will check with the supplier and get softer material. I may even get some brass if I can find localy.


Thank you very much

Philip

Please Log in or Create an account to join the conversation.

Moderators: piasdom
Time to create page: 0.087 seconds
Powered by Kunena Forum