Feed Calculation, from tool, from material, ?

[neurosis]

Im just curious how everyone is doing this and why. Ive played with each and and trying to come up with the most convenient way. When I choose from material, everything works great but it sure takes a while to get everything set up. I figure that I will just try to set up a few separate tool libraries for my materials and choose "from tool" and see if i like that better. How do you do it?

[MultiAxGod]

We have a specific product, so ours is from the tool. The libraries are setup for each machine and speeds and feeds stay the same.

[Mike Whitten CAD/CAM Contractors]

I use "from tool" as I feel that this gives the most flexibility. I always have the material and tools setup so that they will work "from material" though. Since I figure that I am usually going to have a look at the tool data anyways, I just select the "Calc. Speed/Feed" button when I am there. This way, all of your drill type tools are most always correct and you will sometimes only have to make an adjustment or two on milling tools. I used "from material" exclusively for about 2 years in the beginning and found that it seemed too confusing for other programmers to deal with. So I figure that both ways are correct but "From Tool" gives you the best of both worlds.

 

Mike

[Darren Long SPE]

Yep ...from Tool for me too!

A lot of modern cutting tools are designed with specific feeds and speeds in minds, notably the Fast Metal Removal tools. Unless its a tricky material i then manually mod the Feeds and Speeds.

What Ive done is set up tool libraries based on specific types of cutting tools, and then just draw from them.

[neurosis]

I think thats what im deciding on. Im going to set up libraries for the main materials that we machine and use a generic part file to start creating tool libraries using the materials so that once they are done they will work either way. What do you do in the case where the same end mill with the same loc in the same material would have a different feed for slotting rather than side milling or finishing?

[crazy^millman]

I have from tool and have libraries of machines with tools in them, I libraries of Material with the tools in them. I do a lot of different materials and have never really like from Material in Mastercam I have always done it from tool never from Material.

 

HTH

[Mike Whitten CAD/CAM Contractors]

quote:

---

What do you do in the case where the same end mill with the same loc in the same material would have a different feed for slotting rather than side milling or finishing?

---

All you can really do is have the slotting feeds and speeds in the library. I use a main library for all my standard tools. This is large but it covers me for most of the apps.

 

I also do as many others have mentioned and have seperate libraries with specific tools for specific materials with their respective Speeds and Feeds.

 

Mike

[neurosis]

One more silly question. What do you do in a situation where you are slotting and then profiling with the same tool? I notice that if you change your speeds and feeds for that operation, if you accidentally click on the tool again in that operation it resets your feed rates back to what the tool is. Is there a way to lock them in or do you just have to take care not to click on the tool once the operation is open?

[Scott Nordby - Form Tools Inc]

I'm using from tool now. I set up a material called "SFM-IPT" (All speeds set to 100. and all feeds set to 100.) that way I can enter the sfm into the percent field - if you want 250 sfm just type 250 in the percent field and it will calculate it (when you hit the calc button) I also can enter feed per tooth in percent of feed per tooth you can enter .001 for .001 feed per tooth no mess with figuring out precent.

 

I great multiple tools with the same tool number. I may have 3 or 4 tool #1's. and I set he speed for each one for a particular process. when you post make sure you select "NO" when it ask you if you want to add a tool change for multiple tools.

 

Speeds and feed in Mastercam is propably the place I have the most concern about, exspecially as mainly a 2d person. I don't now why they have a finish passes in multi passes dialog box. I can't remember the last time I made finish passes at the same speed and feed as the roughing passes. (Sorry if this sounds like a gripe, its more of a plea to mastercam it improve this area).

[Storkman]

I have been using material for a few years now. I like it. I guess it depends on how many different materials you run.

[Guest CNC Apps Guy 1]

quote:

---

...What do you do in a situation where you are slotting and then profiling with the same tool?

---

Just thinking out loud here but, could you create two identical tools - (different tool desc. to tell them apart) then you could have the best of both worlds. Never tried it but it seems like it could work.

[Mike Whitten CAD/CAM Contractors]

quote:

---

What do you do in a situation where you are slotting and then profiling with the same tool? I notice that if you change your speeds and feeds for that operation, if you accidentally click on the tool again in that operation it resets your feed rates back to what the tool is. Is there a way to lock them in or do you just have to take care not to click on the tool once the operation is open?

---

At this time, the only thing you can really do is Lock the cut( select cut and hit L). I will always put a note on the cut like: ****XY feed 25**. This way I know the feed has been overridden. In older versions of Mastercam, I would also go in the tool and put the slowest feed that was used on the tool for some extra safety. In the recent versions, this causes it to change all the cuts so they all go dirty. I was hoping that the "User Defined" feed calc method was going to fix this issue but it never panned out for me. I was hoping for a function that would disconnect any type of feed calc. This would be kind of cool as you could just select this function when the job was completed. This way you could play with feeds and speeds and not worry about this issue. The big issue with "User Defined" is that it inputs the default "User Defined" feeds and speeds on every new cut. It must just be for Router or Wire People as I do not see a use for it in Mill. Mastercam works pretty good the way it is, you just have to get used to it.

 

Mike