How do you set up your tools (speeds/chip load) while programming?

[neurosis]

I got to thinking about this last week after creating the topic

 

X7 SPEEDS AND FEEDS CALCULATOR BROKEN AGAIN?

 

 

It seemed strange to me that I was the only one that noticed that this thing was broken. The same thing had happened in X3 as well. It didnt seem that anyone had noticed or had been affected by it back then either.

 

That made me wonder, am I the only one that uses this thing?

 

I use this calculator to set the speeds and feeds for every single tool that I use while programming in Mastercam. So when it breaks it is a huge inconvenience to me.

 

Having thought about this a little more, I started to get curious about how others set up their tools for use inside of Mastercam.

 

Does anyone use that calculator? Do you set your tool data some other way? Is there a more efficient way to set your tool data?

 

So my question, How do you guys set your tools data (sfm/chip load)?

[rogkick]

I create the tools and save them as I use them, generally using manufacturers information, and when I import them back in, they remain the same.

Also, generally, we use either high feed aluminium cutters or high volume steel cutters, so parameters never change really. Maybe a manual edit in an operation, if the application is a bit odd.

And...

I never use that feed/speed calculator.

[RonC.]

Same here as rogkick...

our machine keep same tools in them which I I've gone thur and set for alum.soft steel, stasinless 303,304 brass and copper..

if any thing other than that comes in i tweak tools as I pull them in at that point..

 

by the way our machine hold 220 tools..

[neurosis]

I create the tools and save them as I use them, generally using manufacturers information, and when I import them back in, they remain the same.

 

I understand this, but when setting up a new tool, do you use a hand calculator to calculate surface footage to rpm when you get mfg data that doesnt already have the calculations done for you?

 

The built in calculator is very convenient "when it works".

 

It would be nice if you could save the tool data right to the tool from the operations manager.

[RonC.]

I use mfg data .. when ever possible.. :-)

[neurosis]

I use mfg data .. when ever possible.. :-)

 

I must not be wording my question properly. I always use mfg data to set my tools. Then adjust when the situation calls, ie: rigidity, thin walls, etc. (i even use the built in calculator to make those adjustments as it is easier to save to the tool on the fly).

 

Most of the tools mfg data are in sfm and chip load. How to you calculate that data in to rpm and feed rates? Do you sit there with a hand calculator to set your tools up?

[RonC.]

yes I get my speed and feed from mfg. and use a hand held calculator to convert sfm and chip load

to enter them into tool library.. sorry if I miss understood what you was asking... :-)

[gms1]

Almost every toolpath has the ability to do those calculations for you now Neurosis. Instead of hand calculating it I just type .01 in the FPT box and put the sfm in the SFM box and it does it for me.

 

The only exception to this are the legacy amazing surface toolpaths (blend, flowline, contour, etc).

[RonC.]

Now I have use Cimco speed and feed calculator from time to time...

[Brewster]

where I work. we generally are a one-off Aerospace design and build shop. on any given day I could be programming on parts made of aluminum, 15-5 stainless, 304 stainless, A286, Inconel 625, and any other concoction they can throw at us. so it isn't practical (for me) to set a tool library based on materials. I use the speed calculator occasionally, but I have found that it is very limited compared to others available on the internet. It would be great if Mcam could update this feature. until then I will use a third party software.

[neurosis]

Almost every toolpath has the ability to do those calculations for you now Neurosis. Instead of hand calculating it I just type .01 in the FPT box and put the sfm in the SFM box and it does it for me.

 

The only exception to this are the legacy amazing surface toolpaths (blend, flowline, contour, etc).

 

I am aware of that as well. It does not save that data to the tool though.

 

So if I come back to that same tool, or use one of the other operations that you are talking about, I find that I have to start re-entering data. Seems very inefficient to do it that way. I like to set my tool data and then adjust when necessary.

 

Maybe it is time to buck up and start re-creating my tool libraries. I used to have several tool libraries but they corrupted during one of the upgrades and became useless to me. I was so pissed off that I never spent the time re-creating them.

[neurosis]

where I work. we generally are a one-off Aerospace design and build shop. on any given day I could be programming on parts made of aluminum, 15-5 stainless, 304 stainless, A286, Inconel 625, and any other concoction they can throw at us. so it isn't practical (for me) to set a tool library based on materials. I use the speed calculator occasionally, but I have found that it is very limited compared to others available on the internet. It would be great if Mcam could update this feature. until then I will use a third party software.

 

I am in a very similar situation. We have a fairly even combination of production vs one-off type work.

 

I became so good using that calculator (repetition), that I can set up my tools very quickly with it.

 

If you dont mind my asking, what 3rd party software do you use?

[Brewster]

If you dont mind my asking, what 3rd party software do you use?

For milling I use a combination of "Helical's Milling Adviser" AND "FSWIZARD" (the online version). For most other applications (drilling, reaming,etc) i use a software called "CutData"

[Rotary Ninja]

Every toolpath is different. I have always machined by ear instead of using manufacturer data or chip load or SFM. I watch the spindle load and listen to the tool. I have a standard set of tools for aluminum and one for steel. When I create a new tool I throw numbers at it that will get me cutting a chip. Then I adjust at the control until it sounds right. Then I save these numbers to the library tool to get me close the next time. From then on I make adjustments in the toolpaths.

 

If I am trying to move a lot of material I may grab the manufacturer data to get me started and I plug that right into my tool parameters. But very rarely is that the numbers I end up with in the control. There are way too many variables. Part rigidity. Machine rigidity. Tool holder used etc. So I don't spend too much time plugging in values that almost certainly will change at the control.

 

For example... I have been using the same 2 flute 1/2" endmills for years. I have times when I run it at 60 IPM and 6500 RPM. And there are times when I am upwards of 12000 RPM and 300 IPM. So no, I do not use the calculator.

[Guest]

When I set up a job, I will pull tools from the "Big" library, modify to suit and save it to a new library. WHile setting up the tools, I do the feeds and speeds manually using Cimco S/F Calculator and Iscar's HMEM SPreadsheet.

 

So the answer to your question is no, I do not use the S/F calculator. Why not? Not really sure. i guess I kind of have a routine and that's part of it. I can't really argue with success at this point.

[rogkick]

Another reason I use manufacturers data, and modify it slightly according to experience, is that it sets a baseline. Some operators will like to tweak it as they see fit, and if its a worthwhile tweak and they can stand over the decision, then its good.

I always choose the middle of a range and adjust, and where possible will look at tool test reports to see what's going on in the real world.

Seen plenty of amazing metal-cutting on ideal scenarios at major tool manufacturer seminars to know that expectations need to be tempered when running or recomending in the average shop.

[neurosis]

 

So the answer to your question is no, I do not use the S/F calculator. Why not? Not really sure. i guess I kind of have a routine and that's part of it. I can't really argue with success at this point.

 

Yes, the routine is what keeps me using the calculator.

 

I only have to enter the sfm and desired chip load. The data is calculated and automatically transferred to the tool. It is fast and convenient.

 

I suppose that I should develop a new routine since this thing is not important to most. It will not receive the attention required to continue to work properly if it is not a popular function.

[Guest]

Don't take what I said to mean it should not be fixed. It's an important function to some, and really if you think about it, it should be considered a core feature even though few use it.

[Colin Gilchrist]

Dave,

 

You should send in any suggestions/enhancements to QC.

 

With the new 'Tool Database' style libraries, you can now create "cut data" pages and apply those parameters to your tools. It is a bit of work to setup, but it works very well. You first need to create different "Material" data types. You can create as many as you like, so you might have "standard 6061", and "thin-wall 6061", both with different FPT and SFM settings.

 

After you define the materials, you can define different "Cut data" parameter pages, with even further options for refinement.

 

When I right-click on a tool in X7, I use the "search for cut parameters" option at the bottom of the list. This allows you to search for a set of parameters. You then highlight the one in the list you want to use, and press the "accept" button.

 

For the default search conditions, there are a few in the search list. You can click on them in the left-hand column and delete the extra filters if you wish...

[Newbeeee™]

Never clicked on that button before

Looks kind of helpful though.

 

To answer your question, we have very similar work and effectively a tool library.

Also we have a word doc with general settings for different mtl that we have successfully used before (talking inco or hard metal and the HS toolpaths really, so DOC's, stepover, rounding radius etc).

Yup - calculator sat on the desk to get fired up when required but I'll give this a go (still using X5 so I assume it works ok )

I have started a xl spread sheet for a tool library for us, but never got around to creating it in mastercam because I knew X7 was going to be way different.

So when I get around to loading it, I'll start creating it then.

[rogkick]

Thinking about it further...it would be great if one could interface with a manufacturers data, for example ISCAR's online catalog/cutting conditions and pull the recommended material data from there.

Suppose it could be done in a spread sheet, but its a time thing. anyway for the OP .... have a look at this:

http://www.iscar.com/ita/MainPage.aspx?sid=59

[within a thou]

I have one library that I have created tools for each material we cut regularly for each machine we have.The cutters are different grades # of flutes helix and so on so why not have more then one it really helps out my operators as well.. I use the calculator and send it to the machine tweak it at the machine to what the machine can handle now when I find the sweet spot on that particular machine I go back to my library and edit my tool accordingly. Takes a lot of work at first but when its done its done.

[drafting3]

i work in the tool room of an injection molding company, so it's rare to have any sort of production run. i typically have to set new tools for every project. i think my 1/4" 90 deg mill/drill is the only tool that i never have to change.

 

because everything i do is "one of", i set new tools every time in mastercam. i choose a tool from the default library, modify it to match the tool i'll use, then use G-Wizard to calculate my speeds/feeds based on each cut.

 

i then go by ear to adjust speeds and feeds, but most of the time G-Wizard gets it right.

[Slepydremr]

I use MCam to figure the feeds and speeds.

 

I have a generic material definition that has "Base cutting speed (SFM)" set to 100, and "Base feed per tooth" set to 100.

 

Then on the individual tools I simply ignore that it says "% of matl cutting speed" and type in the actual sfm, same for the "% of matl feed per tooth", i type in the actual chip per tooth i want.

 

Now the Calc Feed and speed works fine.

[spade117]

When I set up a job, I will pull tools from the "Big" library, modify to suit and save it to a new library. WHile setting up the tools, I do the feeds and speeds manually using Cimco S/F Calculator and Iscar's HMEM SPreadsheet.

 

So the answer to your question is no, I do not use the S/F calculator. Why not? Not really sure. i guess I kind of have a routine and that's part of it. I can't really argue with success at this point.

 

Pretty much that.

 

A whole bunch of versions ago I created "big" libraries for different types of material. When I created them, I used the mfg's data and put that into cimco speed and feed to get the base starting numbers and then just modify based upon other circumstances.