topic Re: Mill/Turn Post Processing with Y-Axis in HSM Post Processor Forum

Mill/Turn Post Processing with Y-Axis

jackwcallen — Wed, 08 Nov 2017 21:08:01 GMT

Hello,

Thought I would try and see if I can get fusion to post cam programs for our mill/turn machines.

I believe my question is the opposite of this one Linked here. I want Y-Axis moves but the post only seems to spit out C-Axis.

I have check, var gotYAxis = true.

Using doosan mill/turn post for fanuc: Linked here.

Attached example part with basic ops, also the program that I get out using this post.

Thanks for any thoughts.

Jack

Re: Mill/Turn Post Processing with Y-Axis

Laurens-3DTechDraw — Fri, 10 Nov 2017 07:03:56 GMT

That's understandable.

The post checks if it can execute it within given limits.

Those are this in the post:

var yAxisMinimum = toPreciseUnit(gotYAxis ? -50.8 : 0, MM); // specifies the minimum range for the Y-axis
var yAxisMaximum = toPreciseUnit(gotYAxis ? 50.8 : 0, MM); // specifies the maximum range for the Y-axis
var xAxisMinimum = toPreciseUnit(0, MM); // specifies the maximum range for the X-axis (RADIUS MODE VALUE)

The problem you are running into is that it needs to go below X center, and by default that is not allowed.

if you set the xAxisMimimum to a lower value. So -100 for example it should produce Y-axis Code.

Re: Mill/Turn Post Processing with Y-Axis

jackwcallen — Fri, 10 Nov 2017 07:43:51 GMT

Fantastic, that's exactly what I was missing.

And as you say completely understandable.

Many thanks

Jack

Re: Mill/Turn Post Processing with Y-Axis

jackwcallen — Sat, 11 Nov 2017 09:23:59 GMT

I'm trying to do a few tweaks to get this post correct for fanuc 18i (Doosan puma 2500y)

The live tooling codes seem to have changed for 32i.

It appears, for Fanuc 32i, M3, M4 and M5 are used for all spindles, and P11 and P12 designate either main spindle or driven tooling. and M35 engages c-axis, M34 diengages c-axis.

For 18i M3, M4 and M5 for main spindle. M33 driven tool CW rotation and M34 driven tool CCW rotation.

M35 stops driven tool and engages c-axis, M5 stops main spindle and disengages c-axis.

I can see in the post that I should be looking around line 275, but can't work out how to change to replace the P11, P12 with M33 and M34.

Also last question, what is interference check? M110 and M111 in post. Can't find anything in the manuals.

Thanks

Jack

Re: Mill/Turn Post Processing with Y-Axis

Anonymous — Sun, 12 Nov 2017 03:07:20 GMT

The interference check is basically an exclusion zone to hopefully prevent you from crashing your turret into the subspindle.

In reality though, I wind up running almost all the time with interference check off (M110) it's **** near impossible to do anything on the sub side without using M110, at least on my machine (Lynx 220 LSYC).

If your machine doesn't have this functionality, you should be able to strip it out of the post fairly easily.

Steve

Re: Mill/Turn Post Processing with Y-Axis

Laurens-3DTechDraw — Sun, 12 Nov 2017 07:05:14 GMT

@Anonymous We had to set the interference area ourselves since the value's it was shipped with was crap.

Re: Mill/Turn Post Processing with Y-Axis

jackwcallen — Sun, 12 Nov 2017 18:34:43 GMT

Understood, that makes sense.

So as you say, I can take that out from the post as it isn't relevant for this machine.

Would you know where about's in my post I could change the output of P11 and P12's for the spindle selection into M3, M4, M33 and M34.

Thanks

Jack

Re: Mill/Turn Post Processing with Y-Axis

design3 — Thu, 12 Jul 2018 13:16:55 GMT

@Laurens-3DTechDraw I am trying to do the same thing with my HAAS ST30Y and the ST30Y post. I tried switching the xAxisminimum to -100 but it still outputs using the c-axis. Am i doing something wrong? Can you help me please?

Re: Mill/Turn Post Processing with Y-Axis

Laurens-3DTechDraw — Fri, 13 Jul 2018 06:50:11 GMT

If it would require going below X-100(mm) you still will get XZC output instead of XYZ.

Re: Mill/Turn Post Processing with Y-Axis

design3 — Fri, 13 Jul 2018 13:04:20 GMT

@Laurens-3DTechDraw this doesn't require going below x -100(mm). I tried putting in -300(mm) but it still outputs in XZC. Any ideas on why? I also attached a drawing of the part. All the dimensions are in inches.

Re: Mill/Turn Post Processing with Y-Axis

AchimN — Fri, 13 Jul 2018 13:15:11 GMT

Can you please share the part including toolpathes?

Re: Mill/Turn Post Processing with Y-Axis

Laurens-3DTechDraw — Fri, 13 Jul 2018 13:16:17 GMT

No idea.

If you share your part with program and current post processor we can try to find out.

Re: Mill/Turn Post Processing with Y-Axis

design3 — Fri, 13 Jul 2018 13:32:50 GMT

Here is the part, program and current post. Let me know if I forgot anything or if something doesn't work

Re: Mill/Turn Post Processing with Y-Axis

AchimN — Fri, 13 Jul 2018 13:41:32 GMT

Unfortunately this version of this post has that setting twice, first in the beginning of the post, second at the end. The one at the end of the file is still set to "0".

This is already fixed in the latest version of the post which is available here:

https://cam.autodesk.com/hsmposts?p=haas_st-30y

Re: Mill/Turn Post Processing with Y-Axis

design3 — Fri, 13 Jul 2018 13:52:42 GMT

Its always something simple. I should of looked for that. Thank you both for the help it is greatly appreciated.

Re: Mill/Turn Post Processing with Y-Axis

grazvydas — Wed, 28 Oct 2020 08:49:30 GMT

Hi,

I am looking for a help about generated Y axis g-code, instead of G12.1. I want to use Y axis, but the mill-turn post always generated G12.1. How to fix it?

Re: Mill/Turn Post Processing with Y-Axis

Laurens-3DTechDraw — Mon, 02 Nov 2020 07:09:43 GMT

Can't open your Fusion file currently.

But I suspect your issue is the xAxisMinimum set in the post.

Cause with these machines you might have enough Y-axis travel but be limited by the X-axis travel.

Yet this is a guess as it totally depends on your driven tool holder length if it truly is an issue for you.