It's called back-spotfacing. There are cutting tools for doing this.

Thank you for that response.

Jerry J.
UGV5-NX11

https://youtu.be/S3Byf5B6FAw

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

Yes. Not often done, because it is slower than spot-facing from the "open" front side, but it is done regularly.

One important different requirement from normal machining is the tool: Normally, pressure from the drill or milling machine "pushes" the tool back into the drill chuck or milling machine taper adapter. More pressure means a better "grip" between the mill and the tool holder and the cutting surface into the work.

For back facing, the energy of each cutting surface on the mill is pulling the back-face mill itself "out" of the tool holder and "out" away of the mill's socket. They make adapters to resist the pulling force, you just have to pay extra to get a back-face tool that you don't use very often.

Timewise, for each back-face hole, you have to take the milling tool holder apart, put the the cutting head through the hole, re-attach the holder and tool, re-attach the tool holder into the mill, pull up everything tight, then start machining. Takes a while if you have to cut thousands of holes.

"Timewise, for each back-face hole, you have to take the milling tool holder apart, put the cutting head through the hole, re-attach the holder and tool, re-attach the tool holder into the mill, pull up everything tight, then start machining."
Look at the video I posted, no tool disassembly needed. The cutting head is moved in or out by the rotation of the spindle.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

Always better and faster when the company provides you enough money to buy the right tools!

Thanks you so much for the responses. It has been a great help to understand this.

Jerry J.
UGV5-NX11

In production I would expect that part to have a single relief cut between the two ribs/gussets rather than two spot faces. In the past we've used a flycutter or upside down facemill from the top, also used a right angle head and endmill to make the cut.

If your multi-axis mill can rotate its head, then you can simply mill "upside down" by pushing up with a short facing tool.

The ones I have used, it is sent through the hole with no spot face tool on it. Then you manually put the spot face cutter on the special spindle and turn it to engage the drive pin or what ever they use. On a CNC it is an interrupted operation that requires manual intervention, that of course slows the operation down some.

CWB1 hits it pretty close. I’d use a ball end mill or radius cutter so there wouldn’t be a sharp corner. Mill between the two holes, make sure the milled area is as wide as required for the spot face diameter.

A very similar question came up in tool making class 40 years ago.

The issue I see from doing a side mill cleanout of the area between the ribs is it isn't what is specified on the drawing and would need to be an approved alternative manufacturing option. You are making the whole flange thinner between the ribs.

The backface cutter in my earlier video is the easiest method and can be done with a CNC.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

Communication between the shop and the engineer is often necessary to prevent the cost of boo-boos from reaching the bottom line, wish I had a tiny cut of the millions saved annually by 5-minute phone calls. Those blind spotface tools are neat but hardly efficient. For maintenance, prototypes, or short-run work it doesn't make much of an impact, but for serial production the OP's image is a very poor design.

We use a lot of these

https://www.youtube.com/watch?v=3X-fV6XUjVI

John Joyce
Manufacturing Engineer

NX 11 & 12.01 Vericut 8.0.3

If I asked people what they wanted, they would have said faster horses

- Henry Ford