multiaxis 4 axis machine with 4th axis tilted

[shazam/TPP]

i have a Fanuc Robodrill with a 4th axis that is currently parallel with the x axis.

is it possible to set the 4th axis vertical on a sine plate, tilting it up 10 or 20 degrees and program a open pocket using one of the multiaxis toolpaths? i'm trying to use a shorter length of cut ball end mill to mill this pocket. i'm at home right now and do not have access to the file, i will upload tomorrow. any opinions in the mean time? guess at a toolpath?

 

edit:  similar to this, i may have to tip it the same way. i have a closed pocket towards the center hub and open at the OD 

 

 https://youtu.be/bLiYL7U7rvs

[mayday]

I think that will take a custom post. I have the same situation and not sure about how to do it

Im looking to have a 4th axis on a tilt table to open up closed faces for surfacing. kind of like a sine plate that tilts.Not sure if it's do-able

[Greg Williams]

If you use a 5 axis post, this would work OK

[shazam/TPP]

this is the part, it actually has multiple cavities around the part but i was just going to make a sub and index.

 

small cavity.stp

[slyym]

i have a Fanuc Robodrill with a 4th axis that is currently parallel with the x axis.

is it possible to set the 4th axis vertical on a sine plate, tilting it up 10 or 20 degrees and program a open pocket using one of the multiaxis toolpaths? i'm trying to use a shorter length of cut ball end mill to mill this pocket. i'm at home right now and do not have access to the file, i will upload tomorrow. any opinions in the mean time? guess at a toolpath?

 

edit:  similar to this, i may have to tip it the same way. i have a closed pocket towards the center hub and open at the OD 

 

 https://youtu.be/bLiYL7U7rvs

Not sure about needing a custom post or not but I know you can go into the machine definition manager and double click the A axis and it gives you the option to tilt it along Y or Z.  I would try that first.

[Matthew Hajicek - Singularity]

If you set your coordinate systems right and set your A axis manually you can just treat it as a 3 axis path.

[shazam/TPP]

If you set your coordinate systems right and set your A axis manually you can just treat it as a 3 axis path.

3 axis won't work when the part is tilted up 20 degrees. the bottom side of the cavity is slightly hidden needing the A axis to move slightly  to allow the ball mill to cut it properly.

i trying to use triangular mesh toolpath with little success.

[bd41612]

I don't know about the tilt if it will work for what you are trying to accomplish.  We had a situation like that a while back and our reseller said that it couldn't be done.  So I did up a 5 axis post that only allowed 1 index in B axis and put that value in a comment that stated how much to tilt the sine plate, any other index triggered an error message.  From there it was all 4 axis motion with the B axis stationary.  I also did one that used only a manual index on a 3 axis mill for simpler stuff.  This is very do-able, it will just take some time to get it there.

[civiceg]

Why not just tilt the part so you can achieve the best stubbed loc/ out of holder and surface the whole thing? Then hit the one area that is undercut with a lollipop mill, and just use the indexer to index no full 4th. 

[shazam/TPP]

i have made the part in straight  3 axis waterline milling successfully, but the tooling is expensive. using 13 end mills to mill this, all 1/32 ball mills ranging in length of reach from 3x to 8x. the material is Haynes 188 and i would like to just use a 1/32 ball mill with flute length of .093, there are a total of 58 cavities around the part equally spaced. i modified the solid to show just one cavity since my thought was a sub program.

 

BD41612 did you modify the post through the machine def, and control def, or did you actually edit the post? i'm currently tinkering with the MILL 5 - AXIS TABLE - HEAD VERTICAL.MMD, the GENERIC FANUC 5X MILL.CONTROL-9, and the GENERIC FANUC 5X MILL.PST

 

thank you all for the input/ideas!

[CJep]

Whada you think of this here?

I used morph between curves, TAC using a chain, 4 axis output, 5th locked at 20deg

[shazam/TPP]

CJEP    That's what i've been looking for, looks pretty damn good. i will  have to play with it a little but other than that, i owe you sir.

[CJep]

CJEP    That's what i've been looking for, looks pretty damn good. i will  have to play with it a little but other than that, i owe you sir.

 

I like just about anything from the "Founders" brewery and Fuente Hemingway series cigars,...

[shazam/TPP]

those sound really good about now lol thanks again!

[bd41612]

I used the Generic Haas VF-TR_Series 5X Mill.pst that is part of the Mastercam install with the same name machine definition, and I took it from there.  All the functionality of the 5 axis work, just 4 axes can move.

[Jayson Kramer]

Cjep did you post what you did as it still moves the Baxis to. wear you want that axis locked to 20° just thinking out loud.

[CJep]

Yes, with the 5axis post I noticed some B moves less than 1deg

I tried a new file with the 4 axis Gen Haas loaded, I set the tilt angle in the A axis properties to 20deg

 

[shazam/TPP]

Cjep, i assume the toolpath should be in 4 axis. also how did you com up with the chain for the tool axis control?

[CJep]

the TAC chain is the edge curve from the right, xform rotated somewhat close to the center of the pocket then translated in Z 0.125

 

oh poop, I just noticed it got switched to 3, yes it should be 4 axis