Posting to Doosan y-axis mill turn, output is polar coordinate instead of axis milling

[phillip.sheridan]

Hi, I'm new to Fusion, trying to post out to a mill/turn. My part has a milled feature, when I post out it is formatted for polar coordinate interpolation instead of x/y milling. I'm using the library Doosan post. It has " gotYAxis = true" in the function definitions. The part is within the machine +- y axis stroke, and x+- axis stroke. It seems as though I'm missing something really simple. The part model was sent to me by a customer.  Attached is m file, any and all suggesttions are appreciated. 

Link to project:

https://a360.co/3afOU5q

Phil

[Anonymous]

When tool crosses X0, polar mode is triggered in post. I split the surface at X0 and produced rough and finish toolpath output for each half, bypassing polar mode.

Attempt to leave less stock for finish profile failed to produce roughing toolpath so I ended up with few sketches.

[Anonymous · Accepted solution]

Just noticed one face was not finished, here is a fix.

[Anonymous · Accepted solution]

In other threads related to C or Y axis output, some posters altered post to change X0 to something like

X-1. which prevents post from triggering polar mode when tool crosses X0.

Since there is some usable stroke below spindle centerline that varies by make and model, this can be alternative solution for small parts within machine's range.

The question I have is, since polar mode relies on rotating C axis around X0, what happens when you use up your Y axis stroke and only option left is polar mode ?, my guess is failed tool path.

When features are symmetrical, by original design or by intended selection, forcing Y axis output is possible by programming only features above X0, then using circular pattern to rotate C axis and complete rest of the work, just wanted to throw that out there.

[phillip.sheridan]

The Doosan post has several machine choices, within the "puma" section I changed the x axis limit from zero to -50mm as suggested in this answer. The specific 90 degree  milling head in the machine (Puma 2600SY) will go to -57mm, (as in the spec on the mill head ). The post output then changed to xy, instead of xc. No changes were required in the machining operation parameters. I believe you are correct as far as XC polar, when I need that feature, I will have to go back to the unmodified post. Hopefully I won't have a part that requires both😐

Thanks for the help🤗

[Don.Cyr]

I had inquired about this in the past but didn't follow through as I haven't needed it much recently. Seems the Haas post gives you the option of using polar vs X/Y coordinates and I have used that in a pinch just to generate toolpath code and edited the rest to work.. Maybe someone can integrate that code from the Haas post file into the Doosan post?

[Anonymous]

Disabling polar interpolation in user parameter of Haas post results in XCZ output which drives X axis below X0.

If part feature is larger than available stroke of X axis below center line, you have a problem.

Idea is to force use of Y axis instead by one of the methods described in above posts, when you run out of Y axis stroke, your only other option is polar mode, which tends to leave tool marks on center line because tool stops and waits for C axis to rotate before continuing the cut back in positive direction. 

One way to minimize the tool marks in polar mode is by leaving small amount of stock and repeating finish pass, making tool pressure and deflection negligible and less evident.