Lead-in/out from Fusion360 causing issues on VMC15XT

Thanks for the help in advance!

I have a VMC15-XT that is new to me. I started by running a quick test cut, a simple 0.75" cube using Fusion360's generic Fadal post processor. I'm getting an oddity at the entry/exit point of the cut.

All dimensions are spot on at 0.7500" EXCEPT between the start of the cut and the corner. It's obvious to see in the picture attached.

It's 0.050" leftover that's not being cut. It's consistent and repeatable.

To make it more confusing, I did an identical cut, but had the entry point on the y-axis face, and the same problem happened on that face.

I've checked and rechecked my backlash values, also checked my thrust bearings and those are both good. I've also checked the gcode, and it seems fine.

I'm wondering if this is a post processor error, or if there is something off mechanically with the machine. Any help or guidance is appreciated.

Hi,
I use Fusion360 and have not had that problem.

It looks to me like you are using MultiplePasses....is that correct? The shape final shape of the object looks to me like the machine has done the first pass but only partly completed the finishing pass.

May I suggest either turn off the MultiplePass option, and leave StockToRemain at 0.

There is suggestion also that the LeadIN/LeadOut is playing silly buggers with the toolpath. May I suggest experiment with Ramp and turn off LeadIN and
LeadOut. I usually use Ramping toolpaths, in part because I do quite a number of circularly interpolated small diameter holes with even smaller endmils for which
LeadIn/LeadOut would mar the hole, but have now just become accustomed to using it eslewhere.

Craig

Thanks Craig.

Correct, I was using multiple passes, but it persists even with a single pass. (no finishing pass, just one go around) It's as if the lead-in stops short by 0.050" and then everything runs perfectly fine. Wasn't sure if the circular interpolation values were correct, but I double checked and they are.

I can follow the cut with a full finishing pass and be fine, but wanted to make sure there is no mechanical issue that could be causing it.

The ramp is the way to go for holes/bores, but what about contouring?

Hi,

Quote:

---

The ramp is the way to go for holes/bores, but what about contouring?

---

That's where I use ramping....on Contour toolpaths.

Craig

Quote:

---

Originally Posted by joeavaerage

Hi,

That's where I use ramping....on Contour toolpaths.

Craig

---

That would solve it. I'll play around with ramp.

I'm still curious why a simple contouring cut wouldn't work. Doesn't this seem like odd behavior? I've attached the gcode to show that it should be cutting that portion. At line 60, N250 is where it starts the cut that should be removing that material.

If this is a nuance to Fadals, I'm ok with that answer, but want to make sure there isn't something greater at play.

Contour cuts have a setting for pass extension and or overlap. Remember that the path is calculated from the center point of the tool. The tool is round so when the center of the tool reaches the end of the cut there may still be material at the lead in and lead out point that the outer diameter of the cutter never have touched.

Quote:

---

Originally Posted by Kenny Duval

Contour cuts have a setting for pass extension and or overlap. Remember that the path is calculatied from the center point of the tool. The tool is round so when the center of the tool reaches the end of the cut there will still be material at the lead in and lead out point that the outer diameter of the cutter never touched.

---

...x2 Overlap

or try N40 G4 P0

or maybe....Fadal G8 Mode normally does not stop at the Commanded exact position programmed. You might try using G9 to see if, that is the problem, but that would cause other problems like tool marks and is slower.

...x3 on overlap.
also, measure your tool diameter using a tool setter and make sure the value is correctly input into the tool library.

Quote:

---

Originally Posted by everettengr

...x3 on overlap.
also, measure your tool diameter using a tool setter and make sure the value is correctly input into the tool library.

---

I appreciate the help, but I'm being a little thick today and maybe I'm missing something. I've attached a picture of what's happening with the cut.

I understand that that you can overlap the cut to eliminate any starting cut marks, but what it's doing is not cutting the first portion after entry. But then is following the cut path correctly on the backside, which leaves half of one side uncut by 0.050".

The picture shows the top view of the piece after machining.

If I make the entry from the y-direction, same thing happens, just on the y-axis face.

if you are willing to share your file i can post process and check the toolpath i get.

Quote:

---

Originally Posted by everettengr

if you are willing to share your file i can post process and check the toolpath i get.

---

Happy to! Nothing special here, just a 1" initial stock, going down to 0.75".

Thanks!

looks like it should run fine???
i changed to my 1/2 roughing and left everything else the same.
i will run it later this afternoon and check my results.
attached is my post which you can compare to yours.
try running my file, you will just need to move your 1/2 end-mill to T10, or change the tool in the .nfc file back to T2.

https://www.cnczone.com/forums/attac...d=468792&stc=1Attachment 468792Attachment 468794

Thanks for the help. No need to test. I got back to the machine and ran 2 more cubes. They're off by 0.005" not, 0.050". Rookie...Wrote first post from memory.

Everyone was correct, it was overlap and my previous values were wrong. If I overlap just slightly, it solves the whole issue.

Is it best to mark through and edit the post? Or leave as is for the next person. Might be able to save the next guy time so he doesn't have to read through my mishaps.