CNC feed rate and spindle speed

[misc.garfield]

Dear all,
5 months ago, i have joined a company which fabricates plastic parts and my position is product development.

however, the 2nd week after i joined, they transfer me to process department. at here, i have to involved in CNC, cad/cam. before this, i know nothing of cnc and cam.

now, i only relied on the software (alpha cam) to generate the g code.
Several parts have been fabricated/cnc cut using the g code which i created.

however, i found that the products or the result were not so good.

and the spindle speed and the feedrate which i set was always modified by the operator of the cnc machine.

is the feedrate and spindle speed can affect the outcome of the product?
if yes, then how are we going to make decision on feedrate and spindle speed to be used?


i am really new in this field. i will appreciate if someone can provided any tips and or way that can improved my cnc and cam skill.

thanks

[cam1]

Hi:
Talk to the operator, and ask him for some feedback on the speeds and feeds he is using (his input is invaluable). Use those as a starting point. There is alot of info available from the materials manufacturers on the suggested starting speeds and feeds for milling and drilling.
The Machinery Handbook is also a very good reference for speeds and feeds.


hope this helps

[ataxy]

well for one there are basic cutting speed that are used to calculate feed and speed but those may vary from one place to another here are some basic line

first and foremost the tool used to cut the material (coated vs noncoated - carbide vs hss - 2,3,4,5,6 flutes etc....)
the material it self (type of material - thickness of it etc...)
the machine itself (the size of the machine and built)
and also the setup type

the good combination of those for the job you are doing will give you your result now i havent work on plastic much wether lexan or polycarbonate or whatever type it is but you definitly as cam1 said ask the operator for some feedback it as often happen to me to see the engineer and programmer wonder why the part look bad and not asking the operator is point of view wich is a non sence as this would be like ferari not asking michael schumacher if he as an idea as to why the car is not doing its job

[dapoling]

When it comes to feeds and speeds along with what others have responded with you can find a starting point and then the setup man or operator will need to adjust some but not all the tools.
This has to do with the shape of the part, clamping, length of the holder and the tool.

A safe point to start is 4 X SFPM (Surface Feet Per Minute)/Diameter of the Tool = RPM
For plastic I would start with .003 X Number of Flutes = Feed Rate.
Use 2/3 width of cutter for step over cuts and 1/3 diameter for Z depth of cuts.

You will be able to adjust safely up from there and be aware of possible melting in to Heavy of Cuts and RPM's.

[misc.garfield]

Thanks for all your opinions.... communicate with the operators is one of the effective way.

anyhow, theoretical calculation of the feedrate and spindle speed is required. i will appreciate if you guys can provide some study material on this.

dapoling~
we are using vacuum system to suck the material instead of clamping.

when talk about melting, i meet this problem frequently . especially when i cut the part which doesn't required chamfer.

does this melting issue directly cause by improper feedrate and spindle speed?

or can i said that if suitable feedrate and spindle speed was set then melting will no longer happened?

[dapoling]

Originally Posted by misc.garfield Thanks for all your opinions.... communicate with the operators is one of the effective way. anyhow, theoretical calculation of the feedrate and spindle speed is required. i will appreciate if you guys can provide some study material on this. dapoling~ we are using vacuum system to suck the material instead of clamping. when talk about melting, i meet this problem frequently . especially when i cut the part which doesn't required chamfer. does this melting issue directly cause by improper feedrate and spindle speed? or can i said that if suitable feedrate and spindle speed was set then melting will no longer happened?

I do not know what SFPM rating for the plastic you are cutting but a genetic way to calculate RPM=4*SFPM/DIA of the tool which more the likely your machine will not be able to reach those RPM'S do to the SFPM are probably pretty high.

The melting issue has a few factors such as RPM, FEED, Depth of Cuts and are you using coolant or air or a mister for that fact to help cool the tool and chip.
I normally stay around the 5 to 7000 rpm.
With this beware of chip evacuation especially on smaller cutters do to evacuating chips effectively and will melt to tool or back to the part, this would require a reduction in RPM and appropriate FEED.

When trouble shooting problems that deal with RPM and FEEDS always calculate what your changes are so you know where you are and where you have been, to many play the guessing game and unknowingly cover the same ground again with the same poor results.
Always calculate your feed rate by tooth so you know what thickness your chips will be (5000*.003*2=30.IPM) melting, then increase your feed to .004 per flute and look at finish if still melting then drop your RPM and recalculate your FEED with your new RPM, this changes one variable at a time.