Poor surface quality

[Anonymous]

Hello everybody. I can not help but overcome the problem. When finishing on a 3 coordinate machine with a Ø10 spherical milling cutter in shallow areas, poor surface quality is obtained. I suppose that this is due to the large location of the trajectory points in this area and the machine operates jerkyly not noticeable to the eye. Spindle speed 6370, feed 1280 mm/min. Tell me what the problem is and how it can be solved. Thanks!

[craig.shipley]

Hi

There could be any number of reasons for poor surface finish.

Is anything showing inside the software?  Do you have the project and can you share it?

First thing, toolpath tolerance, is it 0.01 or less?

Kind Regards

[Anonymous]

tolerance - 0,01

[craig.shipley]

Any toolpath in particular?

Kind Regards

[Anonymous]

Sorry, but did not quite understand the question.

[craig.shipley]

Hi

Inside the PowerMill project you have 9 toolpaths.

You said there is a surface finish issue for the shallow areas, do you know which toolpath is producing the bad surface finish?

Also, do you have an image of the actual surface finish on the part?

Kind Regards

[Anonymous]

Hi!
Poor surface quality is obtained on a 5 path called "Чистовая". There is no actual image, but it is similar to the image shown above.

Below the photo of another detail here is clearly visible. On this form of a shallow cone, sites with a slight decrease in localization and local dimples constantly appear.
I can lay out the project, but later.
Thanks.

[craig.shipley]

Hi

Thanks for the response but would you mind attaching the image(s) as for some reason I can't see any that are inside the message.

Thanks

[craig.shipley]

Hi

"Чистовая" is not in this project unless I am mistaken?  Please see image attached.

Looking at your images of your part, I agree the surface finish is very bad.  I would not expect PowerMill to produce such a poor surface finish and I would suggest that this is an issue with the machine tool itself. 

It is possible that high speed machining codes are not enabled inside the post processor (such as G5 P1000 or G5.1 Q1 R... depending on what your control supports) but I'm not sure if this would fix your issue completely.

Perhaps the ballscrew or something needs repairing on the machine, as it seems the table is bouncing?

Can you tell me:

• What is the machine make and model
• What is the control and version
• How old is the machine (approx)
• Have you used PowerMill on this machine before?
• Have you used any other CAM on this machine before (with better results)?

Thanks

Kind Regards

[Anonymous]

Good time!

1 VDL 600A

2 FUNUC Series 0i-MF

3 The machine is two years old

4 Yes, we work in Powermill

5 No other CAM system used

Could you tell me how to enable these high-speed codes? I will try all possible options to solve the problem.
Thanks!

[craig.shipley]

Hi 

You need to speak toy your machine tool supplier / Fanuc and see what high speed machining codes are available for your control, then have this implemented inside your post processor.

You could try to use the default Fanuc postprocessor that is available from the install on your machine:

C:\Users\Public\Documents\Autodesk\Manufacturing Post Processor Utility 2019\Generic\Fanuc.pmoptz

This looks like it has the high speed mode implemented, so worth a try (careful testing is required).

Kind Regards

[Anonymous]

Good time! Thanks for the advice, I will try.

[Anonymous]

Hello! My surface quality problem was never resolved. Below is an example of machining a tapered surface with a slope of 5 degrees, which is interesting for angles greater than 30 degrees, the surface quality is good. The trajectory is built along a circle, with the placement of points "inscribe arcs". There were a lot of points, I read that the rack simply may not have time to process such a number of points at a high feed and gouges appear due to acceleration / deceleration, so I decided to reduce the feed to 600 mm / min, + I used the function G05.1 in the program, but the result was not pleasing
An example of how my program was organized:

N118 G00 G21 G80 G40 G17

N119 G90

N120 G54

N121 G53 Z0.0

N122 T3 M6

N123 S6366 M03

N124 G00 G90 X0.0 Y11.199

N125 G05.1 Q1

N126 G43 Z150.0 H3

N127 M08

N128 X-115.394 Y-20.792

N129 Z5.0

N130 G01 Z-3.54 F600.0

N131 X-115.369 Y-20.927

…

N32342 G02 X11.855 Y-124.253 I-124.817 J0.0

N32343 G00 Z150.0

N32344 (---------------)

N32345 M09

N32346 G05.1 Q0

N32347 M05

N32348 G53 Z0.0

N32349 M30

%

CNC operation mode flashing AI APC. Tell me what else could be the problem or am I missing something?

[Anonymous]

Hi. With respect. You do not seem to have any thickness for roughing. Your picture indicates that the roughing tool is under pressure and vibration and has penetrated the work piece and the polishing tool could not compensate. It is better to consider some amount for roughness .

[Anonymous]

The conditions of this image are different. Submit the project of this piece.

[gosmann.andreas]

we have exatly the same problem.

on our haas vf-9.

but cant reproduce this surface on our other haas maschines.

so we thought its not a software problem its a maschine problem. but now i see this ....

[Anonymous]

Thanks for your feedback! I attach the project below. In my opinion, the nature of the processing changed because I reduced the working feed, but this is just an assumption.

[Anonymous]

I also began to think that this is a machine problem, perhaps some parameters in the rack need to be adjusted, but this is a mystery to me ...

[Anonymous]

Hi. I also came to the conclusion that the problem is with the machine cnc. I guess your machine is a little old. To solve the problem, I suggest you avoid the movements of G2 or G3. There are two ways you can do this. Either require the post processor to create a G1 program, or use the redistribute command.

[tiago.sousaFRFK6]

Hello in Point distribution change the output type to tolerance and keep arcs, and in tolerance factor put 0.5.