# Fusion Circular Interpolation?

**URL:** <https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469>\
**Category:** Fusion 360\
**Created:** [March 20, 2021, 11:49pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469 "2021-03-20T23:49:50Z")\
**Posts on this page:** 12\
**Page:** 1

<div class="post-metadata">

**Author:** ![eaststreetcarry](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/eaststreetcarry/32/2504_2.png) [@eaststreetcarry](https://forum.onefinitycnc.com/u/eaststreetcarry)\
**Post date:** [March 20, 2021, 11:49pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/1 "2021-03-20T23:49:50Z")

</div>

I was digging through wondering why the programs were massive and didn’t seem to have any arc movements. I found the Fusion buildbotics post processor at r43022 has circular interpolation enabled, but Onefinity’s flavor had it specifically disabled on the next line.

Jump forward a bit and I see that Onefinity’s post processor was [updated just a few days ago](https://cam.autodesk.com/hsmposts?p=onefinity) and now has an option for circles. A lot of my programs are now 10x smaller.

I don’t see any earlier discussion on this. Why was it disabled?

 ![Screen Shot 2021-03-20 at 7.49.01 PM](https://us1.discourse-cdn.com/flex022/uploads/onefinitycnc/original/3X/6/6/66e7016980c5a18c03ee2628d56331e8f913541b.png)

---

<div class="post-metadata">

**Author:** ![cyberreefguru](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/cyberreefguru/32/27385_2.png) [@cyberreefguru](https://forum.onefinitycnc.com/u/cyberreefguru)\
**Post date:** [March 28, 2021, 1:33pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/2 "2021-03-28T13:33:05Z")

</div>

Looks like that option was added in January, though I don’t know why they would enable it by default. Though the description is a little odd - I don’t know what ‘no’ means in this context - should the item be checked or not to get arcs in the gcode?

-Tom

---

<div class="post-metadata">

**Author:** ![eaststreetcarry](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/eaststreetcarry/32/2504_2.png) [@eaststreetcarry](https://forum.onefinitycnc.com/u/eaststreetcarry)\
**Post date:** [March 28, 2021, 1:55pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/3 "2021-03-28T13:55:54Z")

</div>

Unchecked is “no” and if you check it you get g2/g3 codes. I’m not sure this is actually beneficial with the stock controller yet

---

<div class="post-metadata">

**Author:** ![rccoffin](https://avatars.discourse-cdn.com/v4/letter/r/71e660/32.png) [@rccoffin](https://forum.onefinitycnc.com/u/rccoffin)\
**Post date:** [April 7, 2021, 8:27pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/4 "2021-04-07T20:27:01Z")

</div>

I’m looking at the 2021-03-18 releases for both OneFinity and Buildbotics from the Autodesk post library. Both have revision 43242 and looks like OneFinity is a clone of Buildbotics except for the last 2 lines.

Both have the line  
allowedCircularPlanes = 0; // disable all circular interpolation  
According to the Autodesk Post Processor Class Reference this means " Set to 0 to linearize all circular motion and `undefined` to allow any motion.

I’m wondering why this is so? I have seen some reference to fixing the circle problem but this seems a bit overkill.

---

<div class="post-metadata">

**Author:** ![blaghislain](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/blaghislain/32/33736_2.png) [@blaghislain](https://forum.onefinitycnc.com/u/blaghislain)\
**Post date:** [April 7, 2021, 9:14pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/5 "2021-04-07T21:14:18Z")

</div>

Two week ago I had to reinstall everything on my pc and choose version 43242. After that I was not able to run some of my toolpath after reposting them (my 1F was making a very loud grounding nose and loose reference)… The old fusion360 did not have circular interpolation disable.

We noticed that after I re-enable it there was no problem anymore. I informed Onefinity support and they post this… [Fusion 360 and Circles (arcs) (circular interpolation)](https://forum.onefinitycnc.com/t/fusion-360-and-circles-arcs-circular-interpolation/4649)

---

<div class="post-metadata">

**Author:** ![rccoffin](https://avatars.discourse-cdn.com/v4/letter/r/71e660/32.png) [@rccoffin](https://forum.onefinitycnc.com/u/rccoffin)\
**Post date:** [April 7, 2021, 9:46pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/6 "2021-04-07T21:46:24Z")

</div>

> [@Fusion 360 Post Processor (Download Links Included)](https://forum.onefinitycnc.com/t/fusion-360-post-processor-download-links-included/2897):
>
> Updated: 1/18/2021 This is the post processor for Autodesk Fusion 360. [onefinity\_fusion360.cps](https://forum.onefinitycnc.com/uploads/short-url/wgOjkAxg9eEp8Bbb5nQLDtvFOMX.cps) (51.6 KB) Please refer to this link on how to install it: [https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/sfdcarticles/sfdcarticles/How-to-add-a-Post-Processor-to-your-Personal-Posts-in-Fusion-360.html](https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/sfdcarticles/sfdcarticles/How-to-add-a-Post-Processor-to-your-Personal-Posts-in-Fusion-360.html)

This was the PP announced to the forum. Small changes to the Autodesk one.  
//allowedCircularPlanes = undefined; // allow any circular motion  
allowedCircularPlanes = 0;  
circular interpolation was commented out

could you share the post processor that you were using before this update happened. I’d like to compare

---

<div class="post-metadata">

**Author:** ![eaststreetcarry](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/eaststreetcarry/32/2504_2.png) [@eaststreetcarry](https://forum.onefinitycnc.com/u/eaststreetcarry)\
**Post date:** [April 7, 2021, 9:58pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/7 "2021-04-07T21:58:22Z")

</div>

If you search here for onefinity the post processor history is available: [Post Library for Autodesk Fusion 360 | Autodesk Fusion 360](https://cam.autodesk.com/hsmposts)

---

<div class="post-metadata">

**Author:** ![blaghislain](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/blaghislain/32/33736_2.png) [@blaghislain](https://forum.onefinitycnc.com/u/blaghislain)\
**Post date:** [April 7, 2021, 11:50pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/8 "2021-04-07T23:50:53Z")

</div>

The first version I have downloaded was timestamp 2020-12-10 21:52 on my workstation. When I compare with v43008 the only difference is:  
(both file have $Revision: 43008 31731a89b929cfd1a62f827c2b8ebf233f944dc9 $)

 ![image](https://us1.discourse-cdn.com/flex022/uploads/onefinitycnc/original/2X/5/5f6c5f585c8c4a8de786f8545b5c1d395bb1b446.png)

Using the old file produce gcode with G03. The one on the forum don’t

---

<div class="post-metadata">

**Author:** ![eaststreetcarry](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/eaststreetcarry/32/2504_2.png) [@eaststreetcarry](https://forum.onefinitycnc.com/u/eaststreetcarry)\
**Post date:** [April 8, 2021, 12:24am UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/9 "2021-04-08T00:24:48Z")

</div>

> [@blaghislain](#):
>
> Using the old file produce gcode with G03. The one on the forum don’t

I don’t know which revisions you have. Check the top of the file. I have three different ones locally

```auto
  $Revision: 43008 31731a89b929cfd1a62f827c2b8ebf233f944dc9 $
  $Date: 2020-11-17 14:36:18 $

  $Revision: 43221 a5a0aa6a6357c6456920970306b90da5de1f0892 $
  $Date: 2021-03-18 06:51:29 $

  $Revision: 43242 a5a0aa6a6357c6456920970306b90da5de1f0892 $
  $Date: 2021-03-18 06:51:29 $

```

The line you’re pointing to `allowedCircularPlanes = 0;` is what disables G2/G3 and forces Fusion to create lines out of circles.

---

<div class="post-metadata">

**Author:** ![blaghislain](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/blaghislain/32/33736_2.png) [@blaghislain](https://forum.onefinitycnc.com/u/blaghislain)\
**Post date:** [April 8, 2021, 12:34am UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/10 "2021-04-08T00:34:48Z")

</div>

As explained it seem to be a modified version of 43008 but without ‘allowedCircularPlanes = 0;’ line.

The file was probably shared on FB or forum prior the official post. The modified 43008 was the one I used and had no circular problem. The issue appear when I downloaded the current version available on autodesk 2 week ago. I have order 10022 and use fusion for last 4 month only.

---

<div class="post-metadata">

**Author:** ![blaghislain](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/blaghislain/32/33736_2.png) [@blaghislain](https://forum.onefinitycnc.com/u/blaghislain)\
**Post date:** [April 8, 2021, 1:43am UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/11 "2021-04-08T01:43:12Z")

</div>

If you want to see what was the issue on my machine when ‘allowedCircularPlanes = 0;’ is present look at the video for the test-bug project I shared with support. Everything is ok when enable.  
[https://1drv.ms/u/s!AmsqeiSmdvXigbFMemZS2xivRKLhkA?e=Bwc6NS](https://1drv.ms/u/s!AmsqeiSmdvXigbFMemZS2xivRKLhkA?e=Bwc6NS)

---

<div class="post-metadata">

**Author:** ![blaghislain](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/blaghislain/32/33736_2.png) [@blaghislain](https://forum.onefinitycnc.com/u/blaghislain)\
**Post date:** [April 8, 2021, 8:02pm UTC](https://forum.onefinitycnc.com/t/fusion-circular-interpolation/4469/12 "2021-04-08T20:02:38Z")

</div>

Just a follow-up. I have contacted support last week for the grinding issue and circular problem. They contacted me this morning to test the 1.0.8b1.

On my test, the beta 1 fix the problem for linear cornering and linear circle toolpath. I was able to run fast toolpath with or without circular interpolation enabled.

Info provided \> All cornering will run a little slower, because a code change in 1.0.8b1 causes the motion planner to actually enforce acceleration and jerk limits. You lose a little speed, but the machine is actually following the correct path, and not overloading what the steppers (torque) are capable of.
