Haas sl30 c-axis post processor

[theau_combemorel]

Hello, I have a 2007 Haas SL30 with a C-axis and live tools. I'm currently using an ST20 post-pro with settings to use the C-axis and not the Y-axis. The first problem is that if I check "Use Cycles," when drilling with a live tool, it activates the spindle. So for now, the box is unchecked. Then I have a problem with the C-axis speed. No matter what cutting speed I set on a milled pocket, for example, the F will be based on the speed I enter in the post-pro settings under the name "Integrated" High Feed Rate. Basically, no matter the speed of the operations with live tools: roughing, finishing, the linear speed will be the value in this box. However, when drilling, I have the correct Z-axis speed, and then to move on to the next hole, the C-axis will move at the "high feed rate" speed. Do you have a solution? Thank you very much!

[aju_augustine]

Hi @theau_combemorel ,

Regarding the first problem, the issue was likely because the property "Got Live Tooling" was disabled. If you enable it, the live tool will be activated.

For the second problem, I am not entirely sure of the cause. After the first drilling, the C-axis moves in G0 not in G01 CXX F(High Feedrate) like you mentioned. There is a possibility that the retracting/prepositioning of the linear axis (X/Y) is happening at a high feedrate. This could be due to the "High Feedrate Mode/Mapping" option not being set correctly in the operation or post-processor built-in property to "Preserve Rapid Movement." When set to "Preserve Rapid Movement," the retraction/prepositioning of the linear axis (X/Y) occurs in rapid (G0) mode.

If the problem persists, could you share the project and NC file?

[theau_combemorel]

Thank you for your reply. I can show you the file. You can see ''P3000 M133'' and right after C axis in G1 mode. And the feed rate is (built-in) High feed rate.

[aju_augustine]

Hi @theau_combemorel ,

Thank you for sharing the NC and project file. I see the problem in the 2D Adaptive clearing operation where C feeds are at a high feed rate. I have reported this as a bug.

if you have G112 polar interpolation feature on your machine, I would suggest to enable the G112 polar interpolation post property. (The G112 XY to XC coordinate interpolation feature lets you program subsequent blocks in Cartesian XY coordinates, which the control automatically converts to polar XC coordinates)

[recrutementcip64]

Thank you ! I will try out this solution. Do you know if the bug will be patch soon ?

[aju_augustine · Accepted solution]

I don't have an exact timeline for when it will be fixed, but I'll let you know as soon as it's resolved.

[andrea.amilo]

Good morning, @theau_combemorel  and @recrutementcip64 .

I have studied the topic of high feed rates with c-axis  and believe that everything is correct with the post.
Briefly:
the haas post calculates the correct feedrate when the machine is working using the rotary axis C instead of a Y.
The post uses the programmed linear feedrate and the part diameter to convert the feed into a value suitable for rotary motion.
When machining close to the center of the part (as in you example) the calculated feedrate can become extremely high (sometimes approaching infinity) because the tool’s movement covers a very small distance per rotation.
To prevent unsafe feed values, there is a safety check in the post processor: the feedrate is automatically limited to the “High feedrate” value.
If you look at your NC code, you will see that the speed begins to decrease when the tool moves away from the centre.
That said, I believe the post is working correctly.
One suggestion to help with this would be to reduce the maximum speed, as shown below:

I hope that everything is clear.

Please let me know if you have any questions.

Thanks.

[recrutementcip64]

Thank you very much ! U are right ! 

[recrutementcip64]

@andrea.amilo Maybe you can solve my other problem. When posting my program, the code have too much point. My C axis can't deliver clean motion. Using 2D contour will creat a lot of point even for a simple ligne. Can you help me have cleaner G code ? Thank you

I drop the file for exemple.

[recrutementcip64]

On 2D chamfer, the code is clean. There is a ligne for every point of the part.