2D Adaptive Feed

[AllanVarcoe]

Hello,

I used a 2D Adaptive and the feed rates are all over the place for some reason. I'm using the Haas ST20Y post on that machine.
Thanks in advance!
Allan

[Steinwerks]

Hi Allan,

Can you export your project as a .F3D file and attach it here?

[Laurens-3DTechDraw]

It seems you are running in what we call XZC-mode. The post processor calculates the C-angle and X-value. The haas posts automatically switchs to degrees/min feedrate when entering this mode. This is to maintain the correct feedrate on the machine.

[AllanVarcoe]

Hi! Attaching the file now.

[AllanVarcoe]

I ran the toolpath at 50% feed and the .250" end mill was not happy. There is no way in hell that was correct. I'm machining 304SS too btw. Is there is no G code to convert that to Deg/Min freed rate?

[Laurens-3DTechDraw]

Let's tag @AchimN as I believe he was involved with making these posts. He can explain this most probably.

[Laurens-3DTechDraw]

In the mean time check out this PDF.

Page 46 explains this. By default your machine will probably calculate the speed based on a certain diameter given in parameter setting 102.

But that's very inconvenient for machining on various diameters.

Therefore the post outputs deg/min. But you probably have to setup your machine to do so.

It also seems there is a way to set setting 102 from the post processor properties.

[AllanVarcoe]

So you re saying the post is assuming I'm switching to metric and activating Setting 102 just for the one operation?

[Laurens-3DTechDraw]

Where does this metric switch come into play?

I'm pretty lost in your last reply.

[AllanVarcoe]

On Page 46 of the doc you attached it says:

"If one wants the units to be in degrees/minute the Haas lathe must be turned to metric and setting 102 set to 114.5."

[Laurens-3DTechDraw]

Well yes.

Because there isn't really another option because of control limitations. Or you would constantly, read for every line, need to change setting 102.

Btw, The reason the post uses XZC values instead of G112 is another control limitation. If you get close to/through the center of X, Haas control can't handle that. So the post needs to go to XZC.

But looking into the post it might seem you just need to input your machine's 102 setting into the post properties. So the post does some calculation to be correct even though the control can't handle this properly. So what you see is the post calculation the value it needs to feed into the control, so its calculation makes it correct again. At least that's the look of it in the latest posts.

[AllanVarcoe]

Ok, so are you saying the latest ST20Y post will behave normally? I only downloaded toe post a couple weeks ago.

[AllanVarcoe]

I just ran a program I posted from home and it has NONE of these crazy high feeds, the machine is consistently feeding the cutter using XZC axis. I'm at a loss.

Does the new post do this. I am probably using a 4 month old post at home.

[AllanVarcoe]

BUMP!

I need help please! I'm getting really sick of watching these insane feedrates shorten my tool life!

[AllanVarcoe · Accepted solution]

Figured it out!

Just have to turn "Use Polar Interpolation" to YES!
Holy S#!T  I was about to lose my mind on this!

[Laurens-3DTechDraw]

---

@AllanVarcoe wrote:

Figured it out!

Just have to turn "Use Polar Interpolation" to YES!
Holy S#!T  I was about to lose my mind on this!

---

As long as you don't go near the center of the part this works indeed. But I assumed that was purposely turned off because of that.

[AllanRidesBikes]

My cutters weren't even surviving that long! Haha!

I mean, it was starting at 200+ ipm!!! How long would an end mill that is supposed to see 8ipm last?