Has anyone experienced any issues with the arc center not being correct in milling?
I have a 180 deg semi circle and its center is located at x0 y0 but the the tool paths in SW is off and the posted code show the y center being off .0043"
I drive the tool path off the edge of the model and it is off. I created a sketch circle that is concentric to the model and if I cut a full cirlce the toolpath and code are correct?
In the below I have duplicated the operation and selected both so both toolpaths are displayed. One is drive off model edge and the other off sketch. You can see in the first image they overlap. As you approach the top they no longer line up. I can't share the file publicy. I shared it with @jeff.walters.
Was more curious if anyone else was seeing this. I found it by cutting 2 parts and putting them together and they were correct across the split but off .009" the other direction and scrapped the first sets.
@Lonnie.Cady @Steinwerks So the path looks correct in Fusion360? That is the main question I want to get answered.
@Lonnie.Cady 's original problem in HSMWorks(That started this thread) showed a wrong path in the CAM environment. Where now if I understand you two correctly it's mainly a CAM->POST->Machine conversion problem.
So I think we can conclude you get the same scrapped parts but it's a different issue that causes it.
@Lonnie.Cady wrote:
The same problem exist in IJK. That is the start point is technically still out of location. However the center of the arc is explicitly defined by IJK. when using R the center is calculated which is floating in relation to start points.
If that is the case changing the radius that is given to the post would result in the same path as using IJK right? Because when using IJK the machine would just change the radius to fit the start,end and center points.
Laurens Wijnschenk
3DTechDraw
AutoDesk CAM user & Post editor.
René for Legend.
Laurens Wijnschenk
3DTechDraw
AutoDesk CAM user & Post editor.
René for Legend.
@Vohnsen wrote:
I have never seen this problem.. is is everytime you do circles?
This is a serious problem
It seems to pop-up mostly for half circles I believe. But could technically happen on any radius I think.
Do you run the machines with IJK or R in G2/G3?
You would only see this in R not in IJK.
Laurens Wijnschenk
3DTechDraw
AutoDesk CAM user & Post editor.
René for Legend.
I got the example to look at and the generated toolpath is correct. The R-word issue is unrelated to CAM-4191.
The problem happens because the coordinates are rounded to the requested number of decimals in the post. Commonly 4 for inch mode. And on top of that when using R-word for G2/G3 this will be very sensitive to the rounding. Using IJK is much less sensitive to rounding noise. Based on this IJK is recommended over R. For say 180deg arcs that can give a big deviation at the mid point.
The post engine is only formatting the toolpath to the desired output. It will not try to fit new motion to handle compensation for rounding since it doesn't cannot know the intent of the specific coordinates in the NC program. It would be possible to add code in the individual posts to do various alternatives for G2/G3. Will think about that. I opened CAM-6211 for that.
The R-word issue is not related to the toolpath in Fusion. I can see to R-issue just in an edited NC program.
I have now done the error calculation on the radius due to rounding of XYZs and the error is not significant in itself so it is a combined effect. You can limit the arcs in your post to 90deg when using R-word which seems to avoid the issue.
I'll keep looking at this.
@bob.schultz helped check this also. And we see where the problem comes from now.
Basically some CNC controls will not calculate the correct center when using the R-word. Using IJK-words will have the center specified directly so that wont expose the bug in the CNCs. Which is why we haven't seen that problem before - as IJK is the default for most posts.
The bad center problem can happen for arcs close to 180deg when the CNC doesnt compensate internally for the rounding to the given decimals in the NC program. And as you have seen that can be a huge error.
So what we are going to do is to update all posts to only allow up to 90deg arcs when using R-word. IJK wont be limited and IJK is still recommended. The G-code output is correct as it is for R-word - so if you really wanted to have 180deg G2/G3 support then that could be allowed but it would be up to you to make sure your CNC actually works which will be tricky to test in general. It will be hard to find out what the CNC does in all the possible cases.
There is no away we can know which CNCs will have this R-word problem so that is why we are choosing the safe approach here and setting the 90deg limit for all ISO posts when using R-word.
@Lonnie.Cady wrote:
roughing smoothing deviation =0 this one has correct arc center at 0,0 G3 X4.3313 Y-0.1793 R0.0164 G2 X-4.3313 Y0.1793 R4.335 F60. X4.3313 Y-0.1793 R4.335 G3 X4.3792 Y-0.2313 R0.05 F30. roughing smoothing deviation =.0005" this on arc center is off .0142", .0006" G3 X4.3313 Y-0.1785 R0.0164 G2 X-4.3313 Y0.1785 R4.335 F60. X4.3313 Y-0.1785 R4.335 G3 X4.3792 Y-0.2305 R0.05 F30.
So alright the arc center problem is exaggerated by using R in the code.
But if I look at that code I see the Y is different by 0.0008. That's double the default tolerance.
So or Lonnie set a big tolerance or I would say the path in general is off by more than the tolerance.
But this depens on the line before the first G3.
Laurens Wijnschenk
3DTechDraw
AutoDesk CAM user & Post editor.
René for Legend.
1. The 90deg sweep change in the posts addresses the issue where the CNC would potentially do something different than desired in the NC program.
2. When you use the smoothing deviation feature it will fit in new arcs within the given allowance so in that case you would get different arcs than in the selected geometry. But as long as the visualized toolpath matches the NC program then that is as expected. This is normally used for roughing/semi-roughing where you dont care about the actual passes.
3. So only problem would be if you get toolpath than is wrong for the given settings. If you see this then please submit such examples to support.
Thanks for the example. Makes it a lot easier to review.
The smoothing deviation is not a tolerance. When an operation clears an area it doesn't matter where the toolpath is as long as the area is machined within the given requirements (settings like stepover).
When smoothing deviation is used the strategy will adjust the cutting passes to reduce sharp directional changes within the toolpath. The smaller the smoothing deviation is set to the smaller the less flexibility the strategy will have to fit in a smoother cut. It is kind of like following a race track around and cutting all sharp corners off and the tool can be anywhere on the track. So it is by design that you get different toolpath when adjusting the smoothing deviation.
Not sure what you mean by start and end points not matching since the passes are not connected when generated. Rather the transition linking moves between the passes will be what connects the cutting passes. And the transitions will just move smoothly from one cut to the other. But since the roughing passes are different then the transitions will also be slightly different.
I guess that you could get marks on the parts for at the transitions end point and start of finishing cut when the center can move when using R-word. It would depend on how the CNC interpolates the G2/G3 - if it could overshoot the end point that would be bad. Using IJK would be better since CNCs generally interpolate smootly from start of end of the G2/G3 allowing for a little spiral at the same time. This keeps the motion smooth and avoid overshooting of the start/end points. I guess there is more room for undesired motion when using R-word on some CNCs. I would have expected the CNCs to be smarter and in general do something similar to IJK mode but still with some chance of undesired motion.
I would recommend IJK over R when available. At least we haven't hard about this before and IJK has been the default for most of our ISO posts.
PS. If there where special cases you wanted to test the easiest would probably be to force retracts and use an entry position to force the leads as a particular point along the finishing cut.
Type a product name
