Ti Roughing, Low Rigidity Setup?

[Matthew Hajicek]

Hoping for some advice.  I've got a very low rigidity setup to get this long plate out of the restricted area of the trunnion.  At first I tried my usual 2D dynamic with a Helical ½" EM to get most of the meat off, but it was flexing and chirping as the cutter rounded the ends, Ti being so rubbery, and chipping the tool.  I got it to work by going down to smaller diameter cutters and four stepdowns, but do you think it would work better to do a contour ramp with a high-feed cutter?  Is there another, better option I haven't though of?

Thanks

https://i.ibb.co/hMzmrhg/Floppy-Plate.png">

https://i.ibb.co/MRBZZxt/DF-Plate-Trunnion-Setup.png">

[gcode]

round  the ends first ?

[neurosis]

I do a lot of work like that.  When I have a thin web I never use dynamic. When cuts around the end it causes problems.  

I can trick the tool path in to cutting from one direction but I would have to be at work to show you an example.  

You could always just use a contour path and cut across that in one direction ?

If you're profiling all the way down, do it in steps so it stays rigid.

[Matthew Hajicek]

I emailed Ron, and he votes highfeed.  Got some on order, won't be here in time for this job but I'll have them for next time.

[neurosis]

Thats a good suggestion.  They may still rattle on you at the ends sticking so far out of the clamping area like that.

[BrianP.]

With all those holes have you thought about fixturing it? Drill holes in blank and then mount to fixture. Be able to get really aggressive on a rigid set up. Extra handling could be offset by decreased cycle times.

[crazy^millman]

Yeah I would go with the head style high feed cutter since they hold up better to abuse than a solid carbide if staying with this method. The other choice mentioned is a good one as well. I would leave it tall and mill to a point, but leaving material to keep it rigid. I would then fixture it and cut off the excess like Brian mentioned.

[Matthew Hajicek]

Those holes are tapered double lead threads, might be challenging to fixture to.  If I had a big enough platter I'd lay it down and cut the top or bottom face complete, flip it over on locators, do the other side, leaving it on tabs.  I spose I could make a larger platter sticking way out there.  I only have to make eight parts for now.  Just tweaking thread sizes on the first one and then I can let'er buck.

I ordered a few of these to play with next time:
https://www.helicaltool.com/products/tool-details-82700">https://www.helicaltool.com/products/tool-details-82700

They seem to cost about the same for the whole tool as for a screw-on tip.

[neurosis]

Whats the max depth of cut with those?  about .02?  

If you get a lot of vibration on those ends is going to chip that thing out.

[neurosis]

Don't take my advise to seriously.  I don't own a Haas 5axis.  

If I had to machine that thing with that setup.. I would rotate that down and contour the top with the side of an endmill and then rotate it back up and profile it.  

I don't know how you plan to put those holes in?

[Matthew Hajicek]

If I had to machine that thing with that setup.. I would rotate that down and contour the top with the side of an endmill and then rotate it back up and profile it.  

Essentially what I did, but the other way around.  I did the top view 2D dynamic, then the side view 2D dynamic.  Then 45° and semifinish with a bull, flip for the other side.

I don't know how you plan to put those holes in?

I helix bored them, then I have a custom tapered multi-form threadmill; its the same threadform as on our smaller plates.  Program for double the pitch and you get dual start.  Sizing those out now.

[Matthew Hajicek]

https://i.ibb.co/QQxCJzS/DF-Plate.jpg">

[neurosis]

haha.. that photo really puts it in to perspective.  

Nice job, Matt.

[neurosis]

How do you plan on getting rid of that clamping area?

[Matthew Hajicek]

Thanks!

I'll almost-but-not-quite part it off with a 3mm endmill, then snap it off and sand off the burr.