# Help with rounded sharp corners **URL:** \ **Category:** General Chat\ **Created:** [June 26, 2023, 1:23am UTC](https://forum.avidcnc.com/t/help-with-rounded-sharp-corners/2186 "2023-06-26T01:23:22Z")\ **Posts on this page:** 7\ **Page:** 1
**Author:** ![Lmarti13](https://avatars.discourse-cdn.com/v4/letter/l/2bfe46/32.png) [@Lmarti13](https://forum.avidcnc.com/u/Lmarti13)\ **Post date:** [June 26, 2023, 1:23am UTC](https://forum.avidcnc.com/t/help-with-rounded-sharp-corners/2186/1 "2023-06-26T01:23:22Z")
I tried a simple square profile test case with sharp corners (code below) but the Mach4 toolpath ended up with rounded corners (attached image). Any thoughts on what might be the cause? Lynn Pro4848 ![Toolpath Plot885](https://canada1.discourse-cdn.com/flex027/uploads/avidcnc/original/2X/3/32ec1d6b360aba88efebee55e1ebd76bf1e9cacc.jpeg) G00 G20 G90 G17 G40 G80 G49 G64 G94 T1 M06 (ENDMILL ROUGH) G90 S15000 M03 G54 G00 X2.14 Y9.86 G43 H1 Z1. Z0.2 Z0.1 G94 G01 Z-0.125 F84. Y6.14 F168. X5.86 Y9.86 X2.14 G00 Z0.2 Z-0.025 G01 Z-0.25 F84. Y6.14 F168. X5.86 Y9.86 X2.14 G00 Z0.2 Z1. (ENDMILL ROUGH) G90 S15000 G54 G00 X2.125 Y9.875 Z1. M08 Z0.2 Z0.1 G01 Z-0.25 F42. Y6.125 F84. X5.875 Y9.875 X2.125 G00 Z0.2 Z1. M05 M9 G91 G28 Z0 G91 G28 Y0 G90 T1 M06 M30 % ---
**Author:** ![jjneeb](https://yyz1.discourse-cdn.com/flex027/user_avatar/forum.avidcnc.com/jjneeb/32/244_2.png) [@jjneeb](https://forum.avidcnc.com/u/jjneeb)\ **Post date:** [June 26, 2023, 4:44am UTC](https://forum.avidcnc.com/t/help-with-rounded-sharp-corners/2186/2 "2023-06-26T04:44:51Z")
If you really messed up your Constant Velocity mode settings you could do that, but you would have to be way off from what the standard AVID configuration would have given you for settings. Did you play with any CV or motor acceleration settings in the mach4 configuration lately? ---
**Author:** ![JRG](https://avatars.discourse-cdn.com/v4/letter/j/bb73d2/32.png) [@JRG](https://forum.avidcnc.com/u/JRG)\ **Post date:** [June 26, 2023, 11:49pm UTC](https://forum.avidcnc.com/t/help-with-rounded-sharp-corners/2186/3 "2023-06-26T23:49:00Z")
Is that an outside profile? if inside or on the line that’s what you’ll get. ---
**Author:** ![AncientCowboy](https://yyz1.discourse-cdn.com/flex027/user_avatar/forum.avidcnc.com/ancientcowboy/32/427_2.png) [@AncientCowboy](https://forum.avidcnc.com/u/AncientCowboy)\ **Post date:** [June 27, 2023, 5:25pm UTC](https://forum.avidcnc.com/t/help-with-rounded-sharp-corners/2186/5 "2023-06-27T17:25:11Z")
While the actual result will have rounded corners (the radius of the tool), those rounded outside corners shouldn’t show on the Mach4 toolpath preview. I pasted this code into Mach4 and they don’t show on mine even if I create a tool table with diameters. ---
**Author:** ![Stephen](https://yyz1.discourse-cdn.com/flex027/user_avatar/forum.avidcnc.com/stephen/32/2569_2.png) [@Stephen](https://forum.avidcnc.com/u/Stephen)\ **Post date:** [June 28, 2023, 12:11am UTC](https://forum.avidcnc.com/t/help-with-rounded-sharp-corners/2186/6 "2023-06-28T00:11:48Z")
The rounded corners are not in the G-code. Is your attached image a screenshot of Mach 4? Maybe refresh the view. Sometimes previous traces can stay displayed. Did you try a cut or an air cut, and did it have rounded corners? ---
**Author:** ![subnoize](https://yyz1.discourse-cdn.com/flex027/user_avatar/forum.avidcnc.com/subnoize/32/2197_2.png) [@subnoize](https://forum.avidcnc.com/u/subnoize)\ **Post date:** [June 29, 2023, 4:44am UTC](https://forum.avidcnc.com/t/help-with-rounded-sharp-corners/2186/7 "2023-06-29T04:44:55Z")
Hmmmm, maybe actual pictures would help? ---
**Author:** ![Lmarti13](https://avatars.discourse-cdn.com/v4/letter/l/2bfe46/32.png) [@Lmarti13](https://forum.avidcnc.com/u/Lmarti13)\ **Post date:** [June 29, 2023, 12:33pm UTC](https://forum.avidcnc.com/t/help-with-rounded-sharp-corners/2186/8 "2023-06-29T12:33:18Z")
Thanks for all of the insights. As it turns out, it was complete operator error. I recently switched to a new post processor and missed the fact that G64 was set in the invocation. Mach was set to G61, but was overridden by the GCode file. Since G64 is modal, my subsequent testing of a previous GCode file that did not set G61 or G64 (used the controller setting) also used CV mode (unexpectedly). I removed the G64 in the post processor invocation and all is well. A good learning experience. Lynn