5 axis part help

[Rocketmachinist]

I have this part coming up soon. And to be honest it is a little above my head. I have a general Idea about how to attack this part but any extra input would be nice. I am looking at using our VF4 with the 5axis trunnion. Any ideas about what tool paths to use on this part?

FIXTURE.MCX-6

[crazy^millman]

Rocket let me say it is pretty straight forward. I would probably do some 3+2 work to rough it then only come back to 5 axis on the transitions from walls. Biggest pain will be the .1R in the corners. Might have a .200 endmill made, but would use a .094 and just keller the radii in verses have a customer .200 ball endmill made if I were making a fixture. Looks like clearance so if I could get away with .125 R and use a .25 ball endmill I would. Everything else is just basic positioning and machining from there.

[GoetzInd]

+1 on the 3+2. Look into a tapered ball em to get in those corners.

 

Mike

[michaels123]

To me this is a 4X part.

[GoetzInd]

You're gonna get a lot better finish on the walls and in the sharp corners with tilt IMO.

 

Mike

[Rocketmachinist]

How do I do a 5 axis tool path where the A axis will lock at 59 degrees and I can use a flat cutter to surface the part while the B axis is spinning. I have seen it done online but cannot find any videos right now of what I am looking for. I Did a multisurface 5 axis path that looks like what I want to do but when I post it comes out looking nothing like what It should. Also, how do stop the tool from retracting as much as it does.

[Rocketmachinist]

This is what I'm trying to accomplish but the way it outputs is not right.

[mayday]

Morph between 2 curves. under tool axis control use axis limits and or use tilt angle to lock 1 axis

[Trevor Bailey]

that type of path will be tricky. may need to get your dealer to help out. basically, create a single surface cylinder that runs the length of the part, on the ID. create and edge curve on the back of the part and one on the front of the part, depending on the toolpath you end up with. you can use a few different paths here - flowline, multisurf, paralled to multiple curves(only selecting 1), if you have created two edge curves-morph between curves. all of those toolpaths can be set to spiral with depths cuts.

 

i am heading out, but will be able to get you a sample path later today if you can figure this one out.

[Rocketmachinist]

Thanks that looks much better

[Rocketmachinist]

So i tired to do some simple 5 axis drilling and came across another error. The tool is drilling at A90. and the first hole comes out fine. Then the b axis should rotate and drill again. But the post is making the A axis go to A-90 and in the process trying to crash through my tools. I thought this post was setup to not go in a -A direction but I guess I'm wrong. Any help would be awesome.

 

N4 M11

N5 M13

N6 T10 M6

N7 G0 G54 G90 X0. Y-6.195 B210. A90. S10000 M3

N8 M10

N9 M12

N10 G43 H10 Z2.7205 M8

N11 G83 G99 Z.2189 R.9705 Q.03 F7.2

N12 M11

N13 M13

N14 Y6.195 B150. A-90.

N15 M10

N16 M12

N17 M11

N18 M13

N19 Y-6.195 B90. A90.

N20 M10

N21 M12

N22 G80

N23 M9

N24 M5

N25 G0 G28 G91 Z0.

N26 M30

[mkd]

for the a90/a-90 thing in a 5axis drill path you should set the misc. Values under "additional settings"

 

Secondary axis [0=off, 1=Pos, 2=Neg]

 

set to neg or positive, your preference.

[Rocketmachinist]

Wes,

I have a problem cutting my part using the path that you explained earlier. I cut the part and it is not coming out in a perfect cone shape. It looks like the leading edge was deflecting downwards into the part and creating a spiral shape. The weird part is the trunnion isn't moving, I checked the code and didn't find any A axis moves. All I can think of is my endmill is deflecting but it is a 5/8 carbide and not taking that hard of cut, also the gouge seems to be deeper where it is taking an even lighter cut. I'm using a Raptor workholding dovetail clamp on the part. For the life of me I cannot figure out why this one is happening to me.

[mkd]

got a picture?

we're not talking about the dish on bottom of endmill?

[Rocketmachinist]

No it's dragging the front of the tool and causing a ridge and I think normal endmills should cut flat. I had our photographer take some pics of it, but he hasn't gotten around to sending them to me yet.

[Rocketmachinist]

You know I think you are right, the mills i have have look like they have an angle to releive the center of them. And if I'm cutting only with the ends that would cause my problem.

[Rocketmachinist]

Well I guess I cannot use that method to surface it without using a really small stepover.

[K2csq7]

Standard endmills do have a "dish" to them.

[Rocketmachinist]

Yea most time's it doesn't make a difference until you try and use one like a lathe tool.

[robk]

We do mill turning all the time, and you will leave a cusp unless you optimize the path. How you control the size of the cusp is another thing. Contact your Sandvik rep for a copy of the "Turn Milling Optimization Calculator" or send me an e-mail @ rkielbowicz at grosite dot com and I will send you a copy.

 

Also get free copy of Turnmilling Application guide from Sanvik as well (right through their website).

Ordering code:

C-2920:26

[mkd]

Well I guess I cannot use that method to surface it without using a really small stepover.

 

or get a standard endmill modified into a flat bottom. search catalogs; it is rare but they do exist right out of some catalogs. MSC? robbjack. cant remember...