Centroid Community CNC Support Forum

I have converted a Boxford 250PC and fitted a threading tool on the turret but because the spindle has to turn backward for the tool it will only cut a left hand thread. I cannot turn the tool upside down so the only other option is fit a threading tool in a boring bar and rotate the spindle forwards and cut from the front face like a convensional lathe.
It was supposed to be a M10 metric thread i wondered why the nut wouldn't screw on. DOH

It is because you are cutting a LH thread. If you want to make RH threads with a left turning spindle, cut from -Z to +Z and make sure that the Insert is at the right angle for RH threads.

Use 3000 rpm and 9 passes. CNC should be faster than manual threading and this will give you better surface finish also.

Uwe

Here you go:

suntravel wrote: ↑Sat Apr 23, 2022 4:08 pm It is because you are cutting a LH thread. If you want to make RH threads with a left turning spindle, cut from -Z to +Z and make sure that the Insert is at the right angle for RH threads.

Use 3000 rpm and 9 passes. CNC should be faster than manual threading and this will give you better surface finish also.

Uwe

3000rpm sounds quite fast I will try it tomorrow. So i just tell intercon to start the thread at the -Z end and finish at the +Z end of the job.

tblough wrote: ↑Sat Apr 23, 2022 4:41 pm Here you go:

Thread Turning Methods.pdf

Thanks for the info I will read it and put it into practice.

For M10 /3000rpm it needs 4500 mm/min feedrate, If your lathe cant move at this rate, reduce rpm. Pitch 1.5mm x rpm = feedrate mm/min

Uwe

If you are using Fusion 360 to generate your g code(?), there's a tick box option in the tool library for each tool that tells it which spindle direction is required. I'm not quite sure what you've done but that might be part of the issue.

Presumably you have selected a "right hand" insert for CCW rotation. The difference between a "LH" and "RH" insert is that the orientation of the control points are on opposite corners of the tool - the inserts are mirror images of each other.

You also have to ensure you have correctly defined the direction of the X axis. In Fusion, this is defined in the setup options. Apologies if you have already covered this!

Well I've finally figured it out, certainly for Fusion 360 users.

The setting of RH/LH toolholders and setting the spindle direction is easy enough but the issue is that the X coordinates need to be negative for rear tools. It's already been taken care of naturally but like many things, you can only find it when you know where to look. When you look at the post processor descriptions in the post library or hover over the post name in the dialogue box, you get a popup message that I've simply been dismissing each time: Sure enough, in each tool definition within the tool library, there's a "turret" box. I'd assumed that this was the turret tool number but obviously not, as that's specified elsewhere. Doh. In fact, you need to specify if the tool is in a turret, rack or QCTP. For us, the turret looks right but it doesn't allow reversal of the X coordinate. Selecting "103" provides that negative X coordinate. Ideally, there would be a "turret with -X" option. Obviously for boring bars and drills you'd not want to swap the X coordinate or the spindle direction. Here's what gets posted - note the negative X coords: That spindle direction is also defined in each tool: The toolpath etc shown in Fusion is correct apart from the X axis direction. That's only changed during post processing but you can spin the whole screen 180 degrees to give the "right" view: Thanks for prompting this. I will soon be needing to use this in anger, as my machine requires CW for front / internal and CCW for rear / external tools.

Hope this makes sense (assuming you are using Fusion) and let me know if I've missed or misunderstood anything.

suntravel wrote: ↑Sat Apr 23, 2022 4:56 pm For M10 /3000rpm it needs 4500 mm/min feedrate, If your lathe cant move at this rate, reduce rpm. Pitch 1.5mm x rpm = feedrate mm/min

Uwe

The max speed that CNC12 will allow me to cut this thread is 800rpm. If you try and program it faster it comes up with a Z error saying above maximum and will not continue when it gets to the line of code. Anyway i cut a RH M10 thread except my insert didn't round the top of the thread over. I am searching for a full form insert now.

These boys in Glasgow are pretty good on pricing and fast delivery. I ended up buying 2 each of the metric sizes between 1.0mm and 2.0mm in each of aluminium (AK10) and steel (T250).
https://www.shop-apt.co.uk/threading-inserts.html

I've been using 250rpm and 500rpm for my threading. That's still pretty fast.