[eldzis]

Hello!
I am having problem seting up our 2 axis mill turn lathe in CamWorks.
Our lathe is similar to this one (only difference is that we have a rotating tool crib with active tools):

And I am trying to machine a simple part:

I can easily set up the lathe operations, but when I try to set up milling for the hex part with end mill, it uses more axis than my lathe has.
I want to do the milling with active tool stationary and moving along X and Z axis and the part rotating along the C axis.
How can I force the CamWorks to use my lathe setup?
This is just a test part, in future we need to manufacture simple sprockets and some more complex face milling features.

Can anyone point me to some tutorial, help file or give some advice?

p.s. You can see our lathe here: SIA Metaro

Thanks in advance.

[jame5m28]

Do you have a post specifically written for this machine? Does the machine support "polar" milling?

If the answer is yes to both questions then you will need to select "polar" as one of your operation parameters, it will not simulate this but it should output the code using polar G12 output.

[eldzis]

Yes, our machine supports polar milling (I suppose it does). We bought the machine recently and we are exploring our options.
Our cnc machinist only has some knowledge to program parts on the machine itself, I am working as a design engineer and we are planning to do some more complex parts.
So currently I am reseraching CNC software, to find out which one suits our needs and what to purchase.

Our machinits can program and cut the hex on the lathe itself (the program is quit simple), thus I believe we have a "polar" milling option.
But I don't believe he is capable of programming more complex shapes, that is why we need some sort of CAM software.

So I understand that CamWorks is not capable to simulate polar milling on lathe?
Should I look in to some other software or still try to use CamWorks.
From what I have seen now, CamWorks kind of looks easy to use.
And no, we don't have post specifically writen for our machine.

[jame5m28]

It will simulate the cutting of the hex but not the part moving around,

You will need a custom mill turn post formyourmmachine to get the most out of it,

[CMW-2012]

eldzis, as jame5m28 said Camworks will simulate.

There are a two options you can use "free" or "polar", as jame5m28 mentioned. Both require the post to do the work so it is very important that you have a post.

These selections are located on the NC tab of the operation. You will not see a change on the screen when switching from one to the other. The end result should be the same if the post is correct.

Free-uses XCZ to cut the hex. Free will break the line segements into tiny seqments and output your feed rate in degrees per minute.
Polar (G112)-Uses XYZ and regular IPM feed rates. The polar function (G112) on the control will then take the Y and convert it to C motion keeping the cutting tool in the X positive space at all times. The feed is also converted by the control from IPM to degrees per minute.

Generally polar is your best bet (cleaner code, always in XY positive space, feed rates are IPM).