tool and mtl library

[Elad]

Hi,

I tried to understand the formulas that make the calculations for spindle speed and feed rate from the material.

When i create a new material,i have to insert values (like base cut,etc...)

How should i know what values to add?what is the easy way for building the optimal tool library.

I'm tired of inserting the spindle speed and the feed manualy,somtimes i forget to insert it,and if the worker wont notice this mistake,he will break tools.

James,any recommendations??

Have a great week everybody!

by the way,you have some kind of holiday back the in the u.s??i think it's somthing to do with chicken?? well,i saw Bush on tv letting one of this giant chicken free.

[Hugh.Venables]

Good question Elad. I would very much like to know how all the speeds and feeds are calculated. I right click the tool icon in the tool parameters page of the Operations Manager, then click "Calc. Speed/Feed" at the top RH of the define tools page. For this to work you have to have filled out the Job Setup page, I think, if you want to calculate from material. This generates some very strange speeds and feeds sometimes. Maybe there's a better way?

Hugh Venables.

[Michael Reynolds]

All due respect, but I'm pretty sure that there is no way for mcam to accurately calculate speeds and feeds on a consistant basis. There are too many variables like part/fixture ridgitity, tool hang, coatings, tool geometry, etc.

That's why I do what (I think) Elad does, I have a copy of the Machinery's handbook and a calculator next to me, then adjust the speeds and feeds according to these variables (again, guessing at what I think the tool/machine can handle)

Thanks fer listinin'

Mike R.

[kwolf]

Hi ,

there's are options "% of material cutting speed" and "% of mtl feed per tooth" .The first when multiplied by your raw spindle speed results in final spindle speed and again the second ...

Besides, every mtl has its own base cutting speed which must be multiplied by the % of operation type speed in the material library

Well I hope this helps

[Elad]

Speeds and Feeds are depends on many things,and it's not exact science,but Mastercam still considers the the most importent things when calculatind this values (material,tool dia.,etc...)

I belive that it is possible to configure the mtl and the tool library,and it will give us some kind of reference.even if it's not exactly what we want,it's still better then trying to work with 0 spindle speed and feed

i still think that the way of calculating this speeds is too complicated.

In the mtl library,when i add a new material,i have to give it base of cutting and some more values,and this values will be calculated with the tools parameters.you can learn about the calculation in the help file,just click help in the define mtl window.you'll see all the formulas.

Thanks,

[ 11-25-2001: Message edited by: elad ]

[Hugh.Venables]

Elad, my own MC experience is very short. I always (a dozen times at least!) set up the Job Setup page, particularly select material, and click on Calc. Speed/Feed on define tools page. This way, I never get 0 speed or feed. I am sometimes unhappy with what I do get so I override the generated values with ones I calculate. I am sure the good folks at CNC Software have put a lot into this and would be bewildered by anyone who preferred to manually calculate all their speeds and feeds.

Hugh Venables.

[Elad]

The default values in the mtl and tools library are very wrong.

I always have to change it menualy.

If i have to change it menualy anyway,there is no reason to set the job setup.

I don't know where this value come from,but if we want to try to get close to the real values,we will have to work hard to change the base values in the libraries.

I think the best is to delete this libraries and build it again with your own values.

Thanks anyway Huge,

[Hugh.Venables]

Elad, I'm surprised. The speeds and feeds I get are usually OK. I wonder do you work in metric or imperial (inches, feet, yards, furlongs, etc.)? We work in metric and had big problems initally with feed rates. This was because we were selecting material-meter instead of material-mm from the material library in job setup. The feed rates are then generated in meter/min instead of m.m./min. But I'm sure your problem couldn't be this simple.

Hugh Venables

[Elad]

Huge,

I work in metric too.

I will check again what i do wrong,and i will let you know.

Thanks,

[Guest CNC Apps Guy 1]

The material library I've found to be very helpful. I set it up for OPTIMUM cutting conditions and adjust from there. For example, a Material I made was 7050. The base cutting speed I use is 3000 Surface Feet Per Minute (since you're using Metric, youll need to convert that into SMMPM) and base feed is .0065 Inches Per Revolution. For drilling my feed is 50% of the base and the speed is 10%. You have to do this for every type of machining operation there is. It takes a bit to set up but well worth it in aggravation not felt. Above I sai OPTIMUM, some times I have a weak setup so I need to adjust the speeds and feeds manually but using material is a good way to solve the 0 speed problem.

JM2C

[Luther_Heggs]

Surface feet/min and feed/tooth material ratings are taken from the Machining Data Handbook.

[Hugh.Venables]

James, is that 0.0065" per rev or per tooth?

Luther, is that Machinery's Handbook? If not, could you give us a little more information about what book it is, please.

Thanks, Hugh Venables.

[Mike-T]

The problem I run into is that as the drill dia. increases, so should the "ipr", according to the Machining Data Handbook.

[ 11-28-2001: Message edited by: Mike-T ]

[Glenn Bouman]

Mike-T, you are correct that is why if you check the tool libraries that come with Mastercam you will see that each tool has a "% of matl feed per rev."

For example the 1/16 drill has 1% and the 2" drill has 200%

[Luther_Heggs]

Machining Data Handbook Volumes #1 and #2.

Institute of Advanced Manufacturing Sciences, Inc.

1111 Edison Drive

Cincinnati, Ohio 45216