trochoïdale milling on IGF?

[duivenhok]

Hello all,

I have a simple question (i think).
I have a multus with OSP-P300 control with IGF.
Does IGF support trochoïdale milling or is it that i didnt search good enough today.?

Thanx for now

Similar Threads:

• Novice to milling aluminum, questions about small precision milling
• Haas Toolroom mill CNC Milling machine TM-2 TM2 Milling station Front cover
• Haas Toolroom mill CNC Milling machine TM-2 TM2 Milling station Front cover

[deadlykitten]

hi duivenhock far as i know, igf does not suport trochoidal milling, and this is because there are needed 2 shapes : the shape "before", and the shape "after", and igf can not easy compute the differences between shapes ... if shapes are simple, maybe it can detect the difference ( and run a simple operation ), but otherwise, is not possible ... this requires a more advanced 'islands' algorithm, that can deal with separate, overlapped, partially or full tangent, and common areas, etc; even if this was possible ( good results with organic shapes ), igf would have to adapt it's toolpath inside that custom shape, and this may be a bit too much

just a few more things :
... for simple operations, may be ok to create a soubroutine i just love them, and, if you wish, i may help you to create one
... whatever the programing method, try to use the Hi-CUT Pro, so to smooth cinematic at toolpath joints
... carefull with the tool diameter and cutting specs during climb cutting , so to avoid sending the nut in front of the screw-ball, otherwise cnc wear will be accelerated; climb cutting at high speeds should not create big cutting forces, thus the cutting load should be small comparing to cutting only air : for example, if cutting air requires 30% spindle load, then trochoidal should be 35%eq, not 60%; you may reach 60% with less worries when cutting conventional
... rigid tool, low overhang, etc

kindly

[duivenhok]

Thanks 4 your reply.

What i am gonne do is drill a excentric hole about 60mm diameter 50 mm deep and "spiral it out with a 16mm shaft mill to 140mm (might be that trochoidale isnt the whright wird).
Coudnt find this option in igf so i think im gonne write me a variable program wich i can use in different programmes by just changing the variables.
Im kind of new to milling as i used to work on lathe machines with just some hole making and minor mill operations.
But a man from the tooldelivery company is comming by to get the cutting conditions smoothed but i have to figure out how to spiral outward. But variable programming will do the trick

[deadlykitten]

hello again duivenhok

drill a excentric hole about 60mm

i am afraid that this is not possible; excentric holes requires using the live tool, which is less powerful than the main spindle, and on the 3000 series with radial turets, the main spindle max capacity is circa 60 - 80 mm drilling ( 22-30kw 300-700nm ), and the live tooling max capacity is circa 20 mm driling ( 7kw 40nm )

upper turret live tooling on multus 3000/4000 has 22kw, so please, reconsider, or at least be very carefull, because you may find yourself cutting near the servo torque limit, and that is a dangerous zone

is drill a excentric hole about 60mm diameter 50 mm deep and "spiral it out with a 16mm shaft mill to 140mm

is that a blind or a through hole ?
... through : pls check left side of attached image : use chain drilling, and after that use an end-mill to cut a circle through all those holes, so the middle part will fall
... blind : right side : use chain drilling + plunge milling

this technique is faster then 'only' milling, because drills are designed for such stuff, and also they are more reliable tools, thus there will be less cutting edge wear, comparing to milling

when chain drilling, use a drill that fits very well, so to create a pattern as fast as possible, without too much effort on the live tooling motor

my recomandation :
... through hole : integral ( carbide ) tools : carbide drill + carbide endmill, ; try o14-o16 drill + o12-o14 endmill
... blind hole : indexed ( with inserts ) tools : drill with 2 inserts ( they require less cutting force than single insert drills ) + something to plunge

kindly

[deadlykitten]

just one more thing : if you wish to drill directly with o60 dia + trochoidal turning, you may end up with a bit missalignment on turret A, because high specs may disalign turrets, and also, you will lose time with the trochoidal operation; in short, such an approach will take too much time and will put too much wear on the cnc, and this is why i recomended chain drilling : it is faster, toolpaths are shorter, and will put less stress on the cnc


also, any time you wish, i can help you create a trochoidal soubroutine for simple operations / kindly