Machining open pockets on cylinder

[info99H4D]

Hi All,

I'm trying to machine an open pocket in a cylinder but I'm having a hard time defining the machining boundaries. 

All turning has been done prior to the milling op.  I am doing this on a 3 axis VMC with a manually operated dividing head.  Does anyone have any suggestions as to the best way to tackle this?

[a.laasW8M6T · Accepted solution]

Hey I've had a go at sort of how I'd do it and attatched a file.

I have no idea what work holding you have because you aint gonna mill that just holding it on one end so completely ignoring work holding I've come up with a crude solution.

The key with this stuff is to program your WCS in the center of rotation, then duplicates setups as you go and just change the Z orientation to suit the features you want to machine. then you post out a separate program for each of the different orientations.

Some of the geometry is a bit tricky to pick so I have made some sketches to drive some of the 2d contours how I want them.

See what you think anyway, this is kind of how I do dividing head stuff(no more haha my 4th axis just turned up today yay)

Regards

Andrew

[info99H4D]

Thank you for this.  I was relying on the rest machining option whereas I see you had created a new body for the stock.  I've replicated this in my setup and it seems to be working well with the 3D adaptive now so thank you!  Prior to this I had used a series of 2D contours to get a tool path similar to what I'd use on the manual mill which would work but wouldn't be great.

I've actually got a 4th axis on the machine but I'm fairly new to programming the machine and I think the setup involved with the 4th would be more than it's worth for this as a 1 off part.  Plus I don't currently have the manufacturing extension which I believe would be required for this sort of part?   I'm hoping to get this on the machine over the Christmas period when I've got a bit of time away from production to have a play about.

As for work holding, I've got a threaded plug to hold on to at the chuck end and I'll put a bung in the other for tailstock support.  I've set my boundary to not cut the angled end leaving a ring that I'll take off on the Bridgeport once all the CNC machining is done.

Thanks again for this - I've come from a turning background and the milling side of things has certainly been a steep learning curve!

[a.laasW8M6T]

Yea there's many ways of going about machining a part, I have a particular way I like to do things, but its certainly not the only way. 

I made my own stock solid because I was having problems with the rest machining , I normally would use it though.

In terms of the 4th axis you can absolutely do all of this without the machining extension, you can do positional and wrapped toolpaths, the only thing you currently get with the extension for 4 axis stuff is the Rotary toolpath which you wouldn't use on a part like this.

I've made an example of how to do the 4 axis stuff, you just use "Tool Orientation" in the geometry tab to align the part for machining ops.

I like to group all my operations per tool to save on tool change time as much as possible, so lay things out like using the 8mm endmill for as much as I can then the 3mm then I'd probably spot  and drill, then chamfer and tap.

Again this is just a crude attempt, I would spend a bit more time refining toolpaths and changing strategies depending on what tools I have on hand and tolerance/ surface finish requirements.

Your workholding method sounds great, its probably the best way to do it.

Regards

Andrew

[info99H4D]

Apologies for the delay in my reply.  Thank again for this.  Really interesting to see your use of the 4th Axis.  I've not really looked into this before and I hadn't considered using the tool orientation to control the 4th.  Great stuff!  I've now completed the part but I'm tempted to run another one off just to see how I get on!  I've managed to get the 4th hooked up now so I'm pretty excited to try it out!