Takisawa lathe post issues

[Anonymous]

Hi,I currently using the standard takisawa post available on fusions website. We have a ts-4000y and the post works great except I can't seem to lock out polar interpolation. I want to engage the c axis break and mill with the x and y axis. Anyone have a easy workout? Seems like some deep post editing needed. 

[Anonymous]

Mill/Turn is not vertical mill tipped over, polar mode has its purpose.

Your only option is to program work so that you minimize use of polar mode whenever possible.

I have some examples in link below, ..... but if after reading it you really want to turn polar mode off, search for "gotPolarInterpolation" string in post, change "true" to "false" and save your file.

That will cripple your post and you will not be able to program any work that requires polar mode, your choice. 

https://forums.autodesk.com/t5/fusion-360-manufacture/machine-with-an-axial-tool-using-y-axis-st-10y...

[Anonymous]

For anyone having only C axis machine, turning polar mode off in post significantly cripples already limited capability.

Turning off polar mode will limit your post to programming strait slot from outside to part center line in axial tool orientation and being able to drill and tap holes off center line.

[Anonymous]

Really appreciate your input. It still would make sense to me that in the user defined properties to have a selection to lock c axis. If I wanted to take heavy cuts and engage the c axis break right now I'd have to really cautiously approach every **** tool path. Or I was thinking it would be great just to have something like this in blue as a manual pass through on certain operations...

///////////////////////////////////////////////////////////////////////////////
// MANUAL NC COMMANDS
//
// The following ACTION commands are supported by this post.
//
// partEject - Manually eject the part
// transferType:phase,speed,stop - Phase or Speed spindle synchronization for stock-transfer
// useXZCMode - Force XZC mode for next operation
// usePolarMode - Force Polar mode for next operation
// LockCAxisMode- Force XYZ movement only
///////////////////////////////////////////////////////////////////////////////

[Anonymous]

Posts very in user adjustable parameters, I just wanted to stress the point of not really being able to turn off polar mode entirely.

It has to work the way it does but in some cases you can work around it using different approach in programming work. 

There are pros and cons in everything, if you cut whole hex in one loop you cannot have break engaged so you would want to split stock in few light passes.

If you cut same hex in segments, you could lock C axis and take heavier cuts, unlock C axis, index for next segment and repeat until done.

[Anonymous]

Why couldn't you cut the entire hex with zero c axis movement? The machine has the travel capabilities and only seems limited by the toolpaths and posts (If I were to code it by hand I could do it).

Appreciate your insight though, as I get better at editing maybe I'll try and figure that out. Was hoping someone had already found a work around.  

[Anonymous]

In most cases lathe does not have X axis stroke to walk live tool around center of the spindle so polar mode is used to force tool to work only on positive side of X axis by means of rotating part.

If you have a stroke, more power to you, all lathes I ran so far did not have that ability.

You may be able to do that with small pats, but you will reach limit at some point and it won't be very large diameter.

[Anonymous]

Yes that's one the purchasing points that were made with this machine you have -4" in diameter of X travel. 

[Anonymous · Accepted solution]

I am jealous, it looks like someone needs to revise the way posts are written for specific brands.

In that case, my guess is that you can simply adapt vertical mill program and adjust start and end of a tool path for required codes on lathe.

[johnswetz1982]

So to be clear, your only looking to apply spindle brake clamp> mill your feature using only X/Y/Z > unclamp > Next op. Correct?

[Anonymous]

If I'm following that correctly, then yes! It's one of those issues that 90% of the time won't ever affect anyone. Was just hoping I could have control over that in some easyish fashion. 

[Anonymous]

I failed to ask earlier, what is your machine's Y stoke, I am used to seeing 1.5 to 2 inches in each direction, which depending on tool diameter, poses another big limitation that will shrink the size of part you can mill in that way.

[Anonymous]

Correct. Ours isn't much more. I believe it's a total of 4.7"

[Anonymous]

Yeah, in my experience most parts done on similar machines were below 3 inches diameter and not awfully complicated, usually having threaded holes, slots, hex for wrench or two parallel flats.

In some cases I drilled and tapped axial hole pattern on large parts but not very often.

One thing is for sure, that X axis travel will come handy but don't count polar mode out completely, just program your work in ways that doesn't always trigger its use in post.

If a feature is executable in axial milling without polar mode you can use "manual NC" with "action" and "forceXYZmode" string, you can find some notes on that inside post.

[Anonymous]

Can you elaborate on the XYZ mode. we are trying to figure out how to lock the c axis as well.(its really annoying) and we tried your trick of using the action, but the action doesn't exist in the post, we have a xzc mode or polar mode but no xyz mode.

[Anonymous]

---

@Anonymous wrote:

Can you elaborate on the XYZ mode. we are trying to figure out how to lock the c axis as well.(its really annoying) and we tried your trick of using the action, but the action doesn't exist in the post, we have a xzc mode or polar mode but no xyz mode.

---

I think some posts  have "usePolarmode" or "useXCZmode" so you can force polar mode or XCZ mode with manual NC and "Action" command, but it depends on what you are doing.

I summed up few things in thread below, not sure what you mean by "locking out C axis" but there are ways to limit its activation if you have Y axis.

I am very busy so I am not able to interact on forum at the moment.

https://forums.autodesk.com/t5/fusion-360-manufacture/machine-with-an-axial-tool-using-y-axis-st-10y...