Feed Rates

[troy kordenbrock]

I am milling with mastercam version 9. I would like to slow my feed rate entering onto a part. I am using a square shoulder 1" hog mill. 50% WOC and .100 Depth of cut in 1018 HR. As of now is use 100% tool diameter for lead in and no radius. I want to feed at 80 ipm once I am in the part but only enter at 50 ipm. I know in the lead in/lead out I can change the entry and exit feed rate. I can enter onto the part at 50 ipm but when the machine changes to the faster feed rate once in the part is does so too rapidly and "shocks the tool". Is there any way to make the transition between the two feed rates smoother? Or should I approach enry onto the part a different way? Possibly using a radius or ramping? Any suggestions?

[Tim Simmermon]

I always radius into the part on a contour. There is no way to ramp up the feed gradually, but when you program a radius in it will gradully increase the spindle load.

 

HTH

[Lars Christensen]

Can you use the "highfeed" to do this part?

 

Lars

[troy kordenbrock]

Might sound dumb but, what is "highfeed"? Is it available in mill Level 1?

[Lars Christensen]

Troy,

I am not sure, if it is it would be a button on you right in your operation manager.

It is where you are going to let Mastercam calculate your chip removal rate vers. standard feedrate.

It take a little time to setup, but if you want to use different feeds depending on material removal.

Anybody want to correct me here, go ahead

[mcpgmr]

Try the change at point function. Operations manager/chain manager click on the first chain and right click/change at point. I believe there is a switch in the post that must be on for this to work but I could be wrong. I don't use it. HTH!

[Lars Christensen]

mcpgmr, might got a good quick way here.

You could make your own circle lead in, and then break it in a couple pieces, then just speed the feedrate up as you are leading in.

 

Lars

[mcpgmr]

quote:

---

mcpgmr, might got a good quick way here.

---

Just tried it and it only took 10 clicks including regen. Ran it thru mpfan and it worked. Not too bad.

[Lars Christensen]

Allright I will correct my statement

 

mcpgmr, Has a good quick way

[troy kordenbrock]

I'll give it a shot tomorrow at work. What exactly does the change at point function do?

Thanks

[mcpgmr]

quote:

---

What exactly does the change at point function do?

---

Change at point displays points at the begining of lines and or arcs in which you can pick a slowdown or speed up feed rate along with rpm change or input code before with or after the point at which the change is being made. HTH!

[troy kordenbrock]

Helps alot!

Thanks Again

[88Matt]

It can do even more than that. you can turn coolant on/off, retract/clearance plane (great for jumping clamps), feeds and speeds, etc.. It is pretty powerful but nobody hardly uses it.

 

It is definitely worth while getting to know how to use it; especially if optimizing is a priority.

[Santa Fe]

hey Troy, if you are using V9; on the operation manager select the toolpath you want to edit then right click > options > toolpath editor, here you can brake your chain or single selection to add points, rapid retracts, change feed at centain areas on the chain etc.

 

If you have the mill book there is a section called toolpath editor.