trochoidal machining

[dibz]

Hi do anyone aware of whether trochoidal machining is available in proe?

 

[Zaki]

Hi Dibz


constant_load in volume and roughing type nc sequences are actually trochoidal machining in pro/e and I find it extremely time, tool and machine saving sequence. In simple volume milling the sequence takes 1700 minutes machining time and by roughing it takes only 600 minutes.

 

[dibz]

Hi zaki. but actually pro/e doesnt have trochoidal machining functionality. but it can be acieved upto an extent by as u said constant_load scan type.
but delcam has it. please visit this site also see the video

http://www.mmsonline.com/articles/hsmdm/prog9.html

 

[chf65]

Hi Dibz,


I agree with Zaki. Whether you want to call constant_load trochoidal milling or not, the fact is that the trochoidal milling that you see in Delcam will be in cut about 25% of the time (at best). While constant_load stays in cut 50%+ in the worst case.


Constant_load puts the tool in cutting at its maximum programmed load, and keeps it there as long as possible, before coming out of it. Trocoidal puts the toolin cutting at its maximum programmed load, and as soon as it reaches the programmed load, it starts to move the tool out. I do not see this could be more efficient.


Properly used, constant_load allows you to be a lot more aggressive in step_depth because you do not need to guard against load spikes.

 

[Zaki]

THANX FOR UR FAVOUR CHARLES.

 

[dibz]

Hi thanx to both of u. and can u say me the best parameters setting for achieving this result

Edited by: dibz

 

[Jotry]

Hi All,


Actually NX3 also has trochiodal machining. However, Constant load and other machining parameters in Pro Engineer allows it to be better controlled.

 

[chf65]

Hi dibz,


Here is what I recommend: For a given tool and material, you can be a lot more agressive on step depth than in a typical scan (about 3 times as much) since you will not be getting any load spikes that you must guard against. Also, your CUT_FEED can go higher. Hard to give you specific numbers. Look at recommended surface feed cutting values for the tool and material, set the spindle speed and derive the ideal (most agressive) feed.


I typically set RAMP_ANGLE at 7 to 10.


To speed up and smooth transitions, use RETRACT_TRANSITION=ARC_TRANSITION and set RETRACT_RADIUS to some small value (maybe tool radius).


You will need some trials and errors to find what most works for your tooling/material and machine regidity.

 

[ozamora]

Hi all.


If my control doesn

 

[Zaki]

just make a try and check the mcd file. u can get ur answer

 

[Zaki]

Hi Dibz


u can use open_area_scan and closed_area_scan = constant_load, closed_area_entry u can set this as u like by tengent_helix or ramp or cumbine. u dont need to specify open_area_entry or exit. calculate feed, rpm and DOC as per cutting tool supplier recommendations.