[Joesph Jackman]

default tool path settings are tied to a control definition. do expert mastercam users create a new control definition for different material types and then select the control definition for the material type you need when you start programming a part?

[txcncman]

I am no expert, but I do not get so deep into the set up portion of part programming. I usually do not even bother setting up material type. I do set stock size. I am not so worried about the automatic settings for tool paths because I rely on my experience to input the speed and feed based on my experience with the cutting tool, material, and work holding. Usually takes me less than 10 seconds per cut to input this information, which is negligible in the over all time it takes to get a tool path made.

I can see how it would benefit those with less hands on machining experience though.

[cadcam]

if you are doing by material types then you want to update and create your own material libarys and set the material libary you want when setting up for the next job and tell MC to calcalate from material in the Tool Setup aera.

[Joesph Jackman]

would rather use from tool. what is the best way if i want to stay with from tool?

[cadcam]

So you want it to read the feeds and speeds from the tool setting option using the Matiral libary?

[Joesph Jackman]

want to know if it is possible as well as practical to save default tool path settings by material. by material and tool would be better but i do not see anyway to do this.

[cadcam]

buy tool is the way but you need to set from Matiral to calcalate from the matiral you are using agisnt the tool dia and number of fluts and Matiral of the tool (ex Carbide or HHS)

[Joesph Jackman]

i do not understand how to make the operation defaults get bound to a tool and a material. maybe there is no way to do this and when i start a new part i would have to manually load the operation defaults that i save for each material and a tool library that i make for each material? operation defaults are tied to controls? if so this would make for quite a bit of work because each control would need its own operation defaults and its own tool library?

[cadcam]

Ok I think I am getting confused. so excuse me if I keep trying understand what you want. then I can say yes or no if it can be done. so you want some default settings for some of the operations in the Control defaults that you like to set but it also has to refrence a matrial and certain tools all to be compbined by matrial type.

instead of picking at tool and it setting just the feeds and speeds basd on the tool and matrial? if this tru then I see this being really hard and allot of work.
May I ask what type of defaults are looking for with this? not all just a few of what you are looking for.

[txcncman]

Right. He wants operation defaults (not tool material defaults) for speeds and feeds, regardless which tool will be picked. So, as example, contour tool path will always pick 50 IPM and 500 RPM for both 1/2" carbide end mill and 1/8" HSS end mill.

[Joesph Jackman]

Right. He wants operation defaults (not tool material defaults) for speeds and feeds, regardless which tool will be picked. So, as example, contour tool path will always pick 50 IPM and 500 RPM for both 1/2" carbide end mill and 1/8" HSS end mill.

i am looking to see if it is possible to make saved operation defaults more useful. operation defaults would be more useful if they were linked to a material and even more useful if they were linked to a material and a specific tool. i end up having to do too much editing to my saved operation defaults because they are not material and tool specific. this got me wondering if others had come up with a solution besides not using them.

[cnc-king]

I create different tool libraries for different types of material and in the tool setup page in the machine i set use tool step peck and defaults to come from tool. Feedrates comes from the tool. DOC and Step overs are set from the parameter page. i have much better control this way.

[Joesph Jackman]

I create different tool libraries for different types of material and in the tool setup page in the machine i set use tool step peck and defaults to come from tool. Feedrates comes from the tool. DOC and Step overs are set from the parameter page. i have much better control this way.

Do you have different saved operation defaults identified by material or just one set of saved operation defaults?

[cnc-king]

Do you have different saved operation defaults identified by material or just one set of saved operation defaults?

every machine in the shop have machine specific operation defaults. clearances rapid z position are different on machines depending if they are 3 axis verticals, horizontal, trunion machines, rotary on a vertical mill or 5axis machines and are preset for posting. material depth of cut and stepover is set in the program parameters. feedrates comes from the tool saved in the tool library.

[Joesph Jackman]

so to sum up you have a different tool library for every material you machine. you have different operation defaults for different machines but not different operation defaults for different materials? reason i ask is the step over for 6061 aluminum is going to be different than the step over for inconel 718. you manually edit the step over in your saved operation defaults rather than have saved operation defaults for each material?

[cnc-king]

so to sum up you have a different tool library for every material you machine. you have different operation defaults for different machines but not different operation defaults for different materials? reason i ask is the step over for 6061 aluminum is going to be different than the step over for inconel 718. you manually edit the step over in your saved operation defaults rather than have saved operation defaults for each material?

running X5 i only use the 2d and 3d high speed toolpaths for roughing i keep the step over and depth of cut the same for different materials but kick the feedrate and rpm up or down depending on the type of material. our depth of cut is normally the full flute lenght of the cutter. i will rough titanium at 45 ipm at 2500rpm 1.00 deep with a 5% cutter stepover. aluminum i will run at 475ipm at 15000rpm with the same stepover and depth of cut. tool life is astronomical and wear is uniform.

[Joesph Jackman]

thank you for answering my questions. i will do the same as you and edit the saved operation defaults as needed. what is the reason you do not use the hst finish toolpaths?