New Tormach Post giving empty file!

[Anonymous]

Just downloaded new Tormach Post processor and now when I post a simple operation with 4th axis wrap - the file is empty!

When I post with the Newest Tormach post I get this:

Previous post with exactly the same tool path just different post would give this:

[daniel_lyall]

Where is the post from @Anonymous from fusion or from here http://cam.autodesk.com/posts/ This one I don't know if it has been fixed there is a problem with it doing 4th axis work.

The Generic post from fusion works fine on windows.

[Anonymous]

It was the one me from the tormach site today

[daniel_lyall]

That one is out of date try the Generic post in fusion just make sure you set the rotary table axis in the pre post dialog 

[Anonymous]

Thanks Daniel - the generic post looks good - I am going to try to run it later.  I did notice the feedrates are crazy high like F9999.9999 and I am using inch mode.

[Anonymous]

The generic post didn't work all that great. There were a bunch of errors in pathpilot because it put out G94 moves w no feedrate. There were also some g1 moves with feedrate of F0.

Even worse was that the curves were upside down.

[Steinwerks]

---

@Anonymous wrote:
There were also some g1 moves with feedrate of F0.

---

Were you trying to do a chamfer or engraving with a tool defined as a Spot Drill?

[daniel_lyall]

Yer they had not fixed it then worked this out last weekend.

Try this one it works  It's set up for 4th on the left side of the machine.

[daniel_lyall]

It has G94 and G93 in it, there controller needs a G01 plus free rate on every line there is a G94, A feed was added to all the G95 lines to keep it happy. It looks like they did not fix it the one on the post page is wrong as well.

The one I posted was to get someone going last week. It's bit disappointing.

[Anonymous]

Yes it was a contour w/ a spot drill w/ chamfer settings to 0 i believe.

[Anonymous]

Daniel - the tormach a axis PP.cps post - seems a bit better.

It doesn't post any G94/95 moves.

There are several lines of:

N160 G1 Z0.0394 F0.

Note the feedrate of 0 - but that is easy enough to edit.

I am going to see if the curves are upside down in PathPilot.

[Steinwerks]

---

@Anonymous wrote:

Yes it was a contour w/ a spot drill w/ chamfer settings to 0 i believe.

---

This is because there is no lead-in or lead-out feedrate defined in the tool and you'll have to redefine the tool as a Chamfer Mill to work correctly. While I don't agree with that, it is what it is for now.

[Anonymous]

Well, the bigger issue is that the 4th axis is inverted - in other words it is milling concave vs convex.

[daniel_lyall]

Yep That's the A axis going backwards to what you need.

Grab the A+ post from here this should flip it back over https://forums.autodesk.com/t5/computer-aided-machining-cam/cylindrical-engraving/td-p/6800056

What side off the machine do you have the A axis set Left or right, If it's on the left pointing to the right that A- post should off worked

[Anonymous]

Daniel - thanks for the advice on the other post.  It seems to work pretty

well.  Yes my A axis is on the left of the table as pictured below.

Interesting is that the tool path still looks inverted in the PathPilot window - but in fusion the tool path looks correct 

[daniel_lyall]

@Anonymous can you post the file Brian 

[Anonymous]

http://a360.co/2k2iPlg

Thanks for helping!

Brian

[daniel_lyall]

there was a mistake in your file. you had the origin at the top of the part in the setup, It should be dead center like how you had it in the toolpaths you confused fusion.

Just changing that it looks better in a back plot. File attached for references. 

[Anonymous]

Sadly that wasn't a mistake on my part it was intentional as I didn't think it would make a difference!

I have a lot to learn!  Thank you for kind help Daniel!

It's funny how you see the same folks over in CNCZone and here.  It's a very small world.  Hope you are well in New Zealand!

Hopefully I will be getting my Smithy lathe soon - I will post some vids over in the 'zone.

[daniel_lyall]

And I hope it is working.

For wrapping in fusion not haveing the setup origin and toolpath origin at dead center makes things go nanananna or have them at different places.

It's always the simple things with fusion that can make stuff go Nanananan