Defining Tools

[Justin Beebe at Folsom Tool]

When I try to define my tool in Mastercam V9 so I can have Mastercam calculate feeds and speeds it gives me the same feed and speed regardless of what material type I define the tool as being. It always gives me the feed and speed for HSS even when I define a carbide tool. I do this after choosing the material type from the material library on the job set up page. How can I have Mastercam caculate feeds and speeds for any material tool.

[crazy^millman]

Look on your set-up page and see if it is set as speeds and feeds from tool or Materail.

 

HTH

[Justin Beebe at Folsom Tool]

It is set on from tool. It seems to use the same surface footage for carbide or HSS for example 440 stainless 400BHN uses a 35 surface footage whether I define the tool as carbide or HSS. Should Mastercam automatically change the surface footage when I select carbide or do I have to change the surface footage my self. I would appreciate any help.

[Thad]

I could be wrong, because I don't use these features, but as far as material goes (i.e. your material library), I believe it's referring to the material that you're cutting, not the material the cutter is made of. When you define your tool, you can define what material it's made out of.

 

If you have a 1/2 endmill that is HSS, it's a different tool than a 1/2 endmill that is carbide. Whereas aluminum is aluminum no matter what you're cutting it with. That's why they need to be defined as 2 different tools.

 

I would think that you could call up a 1/2 carbide endmill and based on the material you're cutting, MC would calculate the speeds and feeds.

 

To sum it all up, I would say that when you have MC calulate feeds and speeds by material, you're talking about the material that you're cutting, not the cutting tool material.

 

Welcome to the forum!

 

Thad

[Justin Beebe at Folsom Tool]

Thanks Thad. Your right the material library refers to the type of material your cutting. The problem I'm having is getting Mastercam to caculate a different speed and feed when I switch the cutting tool type from HSS to Carbide. The only way I can get it to work is to change the surface footage value myself. It won't change automatically when I select carbide from the drop down menu on the define tool parameters page. I don't normally use this feature either I am just trying to get it to work. Thanks

[Thad]

quote:

---

The problem I'm having is getting Mastercam to caculate a different speed and feed when I switch the cutting tool type from HSS to Carbide.

---

I see. I understand completely what you're trying to do and seems like a legitimate concern. My only question is how would MC know what to change the surface feet to when you change the tool material? You don't have to answer that, I'm just thinking out loud.

 

A coworker was setting up libraries for soft steel, tool steel, and hard cut. Making them the default libraries for different configs, he now lauches the correct desktop shortcut for the type of job he's cutting. He's on vacation next week but I'll have to ask him when he gets back if he got it all set up and how it's working.

 

Does anyone else who uses these features have anything to add to this?

 

Thad

[Guest]

You need to set this in a couple of places for it to work correctly.

 

In your material library, you need to set each material that you will use with a base SFM

 

Then you set the base chip per tooth setting, now on you rallowable tool material setting you set how each tool material will interact with the base settings. HSS is set for 100% on both, so that means when you set aluminum as material, your base settings are active.

 

But there is a way to tweak them even further.

 

On your tool definition page, you can tweak indiviaul tools to cut based on the base settings in the materail library.

Under no. of teeth there is 2 boxes, % of material SFM and Chip load, those allow you to customize specific tools based on the base setting the material library has.

 

I don't do it this way myself because of the obvious technicalities of getting it all set up but that's the nuts and bolts.

 

Everything is tied to the base settings of SFM and CPT.

[Thad]

I figured one of the professionals would be along to explain it.

 

Thad

[Justin Beebe at Folsom Tool]

Thanks John and Thad that helps a lot. Now I just have to decide if I want to take the time to set it all up. Thanks again