G3 code on one line instead of four lines

[tiborbDDHYR]

The helical code what Inventor creates are too long and we are struggling to upload the generated code. The generated code create four block of codes with 1/4 of the circle in every single block instead of using a simple "G3 I-4." command. This is the program code generated by HAAS generic post processor, but seems like all the one does the same.

G3 X156.385 Y-106.093 Z-0.986 I0. J4.;

X154.382 Y-98.872 Z-1.6 I0.349 J3.985;

X159.084 Y-105.344 I2.351 J-3.236;

X154.382 Y-98.872 I-2.351 J3.236

instead of 

G3 I-4.

[serge.quiblier]

Hello @tiborbDDHYR 

probably because of the setting at the start of the post.

maximumCircularSweep = toRad(90);

You probably have a maximum arc sweep limiting to 90 degree.

As the settings is used for arcs AND helix, depending on your machine capability, you can change the value.

You can either modify the post, or eventually change the value in the post properties.

Regards.

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[tiborbDDHYR]

These are the settings and looks like doing the job with helical contour, I have to check it with boring and threading as well..

maximumCircularSweep = toRad(360)

getCircularSweep()) > 90)

Radius arc: No

maximum circular radius 1000

[serge.quiblier]

Hi @tiborbDDHYR 

Is it possible to share your Fusion file, and the post processor you are using?

This way i will be able to check the parameters but also the function handling arc interpolation.

You can either share a link to your Fusion file. See:
https://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/sfdcarticles/sfdcarticles/How-t...
or you can save an archive (f3d, or f3z) and share it on the forum
https://knowledge.autodesk.com/support/fusion-360/troubleshooting/caas/sfdcarticles/sfdcarticles/How...

Cheers.

[tiborbDDHYR]

This is the post which is making the first several helix with 3 blocks, then using single line helix for the next six or so, then repeating the same to the end of the program...
https://pastebin.com/RsB9WrQV

The post processor is here

https://pastebin.com/uKZAfzu8

[serge.quiblier]

Hi @tiborbDDHYR 

I tried simulating the code using HSM Edit.
The result look strange, but :
1 - i don't know the brand and model of the controler as there is not comment in the post.
2 - i selected a Fanuc analysis, that think that IJK are relative to the start point of the arc and I0, J0, or K0 can be omitted.
3 - as the controler is unknown, i can't tell is missing XyIJ values could be problematic or not.
4 - i have absolutlety no idea what the part look like.

So can you tell me the brand and model of the controler, and share your inventor file, please?

[tiborbDDHYR]

This is the code in simulation and see attached files for the whole nc program and post processor without header.
It is basically a generic fanuc g code.

Thanks

[serge.quiblier]

Hi @tiborbDDHYR 

the only thing noticeable when simulating your latest code, is the starting point on the problematic arcs.

Apparently they are starting either at 12 or 6 o clock.

I am not sure this is the cause, as i can also be due to the model or geometry used for creating the toolpath.

Can you share the inventor file used for creating the g-code?

I will be able to look at the model and try to identify a source cause.

I will also try tomorrow to play with the starting point.

Regards.

[tiborbDDHYR]

See attached file, hope I did the "save as" procedure well.

Also at this occasion the order is just funny and there is no way to reorder it within 2D contour.

We are using Inventor professional 2022 here.

[tiborbDDHYR]

Any news?

[serge.quiblier]

Hi @tiborbDDHYR 

nothing can be done in the post, as the post is reacting normally.

In fact the issue is coming from Inventor.

I outputted your operation using the dumper post.

For the correct helical interpolation, Inventor has sent something like this:

514: onMovement(MOVEMENT_FINISH_CUTTING /*finish cut*/)
514: onCircular(false, -18.06365966796875, -146.99430084228516, -251.10000002384186, -14.06365966796875, -146.99430084228516, -251.10000002384186, 800)
  direction: CCW
  sweep: 360deg
  normal: X=0 Y=0 Z=1 (XY)
  radius: 4
515: onMovement(MOVEMENT_RAPID /*rapid*/)

But on the incorrect helix, it has generated that:

549: onMovement(MOVEMENT_FINISH_CUTTING /*finish cut*/)
549: onCircular(false, 72.73313903808594, -146.99410247802734, -251.10000002384186, 76.73294067382812, -146.99430084228516, -251.10000002384186, 800)
  direction: CCW
  sweep: 89.994754deg
  normal: X=0 Y=0 Z=1 (XY)
  radius: 3.999802
550: onCircular(false, 72.73313903808594, -146.99449920654297, -251.10000002384186, 68.73333740234375, -146.99430084228516, -251.10000002384186, 800)
  direction: CCW
  sweep: 179.994317deg
  normal: X=0 Y=0 Z=1 (XY)
  radius: 3.999802
551: onCircular(false, 72.73313903808594, -146.99410247802734, -251.10000002384186, 72.73330688476562, -150.993896484375, -251.10000002384186, 800)
  direction: CCW
  sweep: 89.999563deg
  normal: X=0 Y=0 Z=1 (XY)
  radius: 3.999794
552: onMovement(MOVEMENT_RAPID /*rapid*/)

3 separate arcs instead of a single one.

I couldn't try to change the starting point or check the model, as the solid is missing from the project:

Cheers

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[tiborbDDHYR]

The solid model attached and the generated code as well, also the cam settings too.
When I select one line of toolpath, it is creating single line G3 but in a funny order.. do not see how we can control it - like x or y way, or selected order, shorter path... nothing there. See program number 1001.

If I selected two rows of contours it is even more strange, plus there is one circle made by two lines of G3.. See program number 1001-2

If we select all the three rows of contours it goes again in a strange way like before and create double line G3 code lines.

If I would make a drill operation, there is an "Optimize order" option at least. See image number 1001-4.png

1001-21001-31001

[serge.quiblier]

Hello @tiborbDDHYR 

i will report the issue to the developers.

Nothing can be done on the post processor side.

Trying to force a starting point may change the order, but there is no way, at the time, of controlling the machining order between the several contours.

Same for the arcs slicing issue, i could not find a work around.

Regards

[serge.quiblier]

Hello @tiborbDDHYR,

please, find some updates on your issues.

Considering the machining order, there is a check box that can improve your control.

As I am not an expert at Inventor, I wasn’t aware of it. (Fusion is like my 7 or 8th CAM system, and I have not even begun to investigate Inventor)

Please note the "Preserve Order" checkbox.

For the arc splitting, apparently the developers are testing some new algorithms, and they seem to reduce this kind of problems.

Regards.

______________________________________________________________

If my post answers your question, please click the "Accept Solution" button. This helps everyone find answers more quickly!

[tiborbDDHYR]

I thought there could be an "Optimize order" option with order by x/y or inside out like we have in the Drilling`s Geometry tab. The reason I would like is that sometimes we have hundreds of features to mill out and select them one by one is just time consuming. Specially if there is a solution for the same problem within the drilling cycle.