Profiling artifact question

[infamous_panda]

Can anyone comment on potential causes for the artifacts shown below. They occur most often during profile milling where the tool plunges into the material. But they also seem to happen when the machine makes an abrupt change in direction.





My setup is a Pro48, 2.2kw spindle, Nema24, Gecko G540, Older PC parallel Port running Mach3. I typically cut plywood and mdf with a Freud 1/4"at 18,000 rpm and 200 ipm. I was using VisualCAM for Solidworks, now using Fusion360 and the issue remains with either post processor.

Similar Threads:

• Question about carving artifact
• G71 internal profiling question
• Need Help!- Profiling Question
• Profiling question in Pro-Nc
• Profiling Question

[toddedwards]

Hmmm, if it is happening on abrupt changes in direction, it may be backlash. Best to slow down the stepping speed and see if it stops happening. On an older DIY machine I built, I found I had to reduce my max speed and steps as the change in direction actually made the whole gantry move a couple of mm creating a divot in the material each time.


Sent from my iPhone using Tapatalk

[klhoard]

.
Have you tried cutting something soft, like pink foam insulation? Perhaps the router bit is digging into the plywood during plunges instead of cutting. Are all your bolts snugged down tight?
.

[109jb]

Are you running in Exact Stop mode or path blending/constant velocity. If exact stop, many controllers actually do stop ever so briefly at the end of a move. If there is any flex in the cutter during movement, this small dwell could result in the cutter un-flexing and taking a little bit more material out. Path blending/cv will maintain as much velocity as possible rather than stopping at the end of each move. For tangent moves it should not slow down at all, but for sharp corners it will slow down only enough to maintain the tolerances set for the path blending feature. This can result in rounding of sharp corners a little depending on the path blending tolerance.

Looking at the first picture it looks like there is a little ramp leading to the biggest part of the divot. This could be where the machine is slowing down going into that junction and un-flexing as mentioned above.

[klhoard]

.
Do the divots always happen at the same place in the cut or at random locations?
.

[ger21]

It's flex in your machine, or tool deflection.
One solution is to never plunge. Always ramp into the cut.
Inside corners will always do that, even with a very rigid machine. You either want to put a radius in there, a little larger than the tool radius, or do a roughing pass first to remove most of the material.

[infamous_panda]

Hmmm, if it is happening on abrupt changes in direction, it may be backlash. Best to slow down the stepping speed and see if it stops happening. On an older DIY machine I built, I found I had to reduce my max speed and steps as the change in direction actually made the whole gantry move a couple of mm creating a divot in the material each time.


Sent from my iPhone using Tapatalk

I tried slowing it to 60%-80% on subsequent runs. There was definitely some improvement although slight.

[infamous_panda]

.
Have you tried cutting something soft, like pink foam insulation? Perhaps the router bit is digging into the plywood during plunges instead of cutting. Are all your bolts snugged down tight?
.

I have, although it was some time ago and there are too many other variables to make a good comparison. I do have to take some time and tune up the whole set up. Check bolts, adjust squareness, tramming etc.

What do you mean by digging vs cutting? Is that something a ramp in would help?

[infamous_panda]

Are you running in Exact Stop mode or path blending/constant velocity. If exact stop, many controllers actually do stop ever so briefly at the end of a move. If there is any flex in the cutter during movement, this small dwell could result in the cutter un-flexing and taking a little bit more material out. Path blending/cv will maintain as much velocity as possible rather than stopping at the end of each move. For tangent moves it should not slow down at all, but for sharp corners it will slow down only enough to maintain the tolerances set for the path blending feature. This can result in rounding of sharp corners a little depending on the path blending tolerance.

Looking at the first picture it looks like there is a little ramp leading to the biggest part of the divot. This could be where the machine is slowing down going into that junction and un-flexing as mentioned above.

Honestly I am not sure, but would like to look into.

Would these parameters be something in Mach3 or the CAM software/post processing

[infamous_panda]

.
Do the divots always happen at the same place in the cut or at random locations?
.

Random per job, but they are consistent with each pass in the same job if that make sense.

[infamous_panda]

It's flex in your machine, or tool deflection.
One solution is to never plunge. Always ramp into the cut.
Inside corners will always do that, even with a very rigid machine. You either want to put a radius in there, a little larger than the tool radius, or do a roughing pass first to remove most of the material.

I think this is definitely something I need to look into further. I ran a job with the a brand new bit but this time I mounted it with minimal amount of shank extending from the collet. Improvements all around.

[infamous_panda]

Can anyone comment on my speed and feeds.

1/4" 2x straight flute carbide bit. 18,000 rpm, 200 ipm, 0.375 depth of cut. Pine Plywood.

I think they are reasonable but...

Also I always have a lot chips remain in the cut path on profile passes unless I reduce my depth of cut to something less than 1/2 the OD of the tool. Is this just the deal with straight flute bits?

[ger21]

I would say the rpm is too high, and with 1/4" bit's, I tend to not cut more than 1/4" deep per pass. Drop the rpm to 15,000. With a spiral bit, I'd lower the rpm even more.
If you are using carbide tipped tools, then they are more flexible than solid carbide.

Also I always have a lot chips remain in the cut path on profile passes unless I reduce my depth of cut to something less than 1/2 the OD of the tool. Is this just the deal with straight flute bits?

It's the deal with any type of bit, but especially with smaller bits. Your dust collection plays a small role here, but it won't help that much. Upcut bits will pull the most chips out, but they can still get packed in. The best way to deal with this is an air blast at the tool.

[infamous_panda]

I would say the rpm is too high, and with 1/4" bit's, I tend to not cut more than 1/4" deep per pass. Drop the rpm to 15,000. With a spiral bit, I'd lower the rpm even more.
If you are using carbide tipped tools, then they are more flexible than solid carbide.



It's the deal with any type of bit, but especially with smaller bits. Your dust collection plays a small role here, but it won't help that much. Upcut bits will pull the most chips out, but they can still get packed in. The best way to deal with this is an air blast at the tool.

Funny the change in perspective, coming from a small Taig milling machine, I always considered 1/4" to be "large". Thanks for the tips, just so happens I installed an air nozzle for the spindle.

[sixstringlz]

Any update? I'm having a simular issues.

[bonesbr549]

I had a similar issue. I reformatted my laptop running mach I did not put virus software on it. I also changed from running gcode file from network. I copy it to local c drive. Do not leave thumb drive in machine. Have not had repeat since