Odd question for my old machine

Hi Guys,

So my machine is old and the Fusion 360 is producing CAM calling for 10,000 RPM on my little 1/8" end mill. I can only go about 3200 RPM on my machine. This means the speeds and feeds are all off in my CAM by 3x at least. What's the best way to compensate for this in my old Tree 200R machine? It's a good and highly accurate machine when it does work but trying to move at the speeds the CAM produced is making my smaller circles "skew" and also very bad for my end-mills.

So is it best to let CAM produce the correct feed and speeds or can LinuxCNC just do it for me? I see there's a "Feed Override" can I just turn that down to 30% and call it good, knowing my spindle speed is about 30% of the desired 10k RPMs?

Greetings,

My machine is also limited to 4000 RPM.

Within the CAM software, look for a tool definition parameter. Set it to the max RPM available and the software should recalculate the feeds correctly.

Cheers,

Dave

fc60 wrote:

Greetings,

My machine is also limited to 4000 RPM.

Within the CAM software, look for a tool definition parameter. Set it to the max RPM available and the software should recalculate the feeds correctly.

Cheers,

Dave

So I did this and the CAM software definitely adjusted the feed rate to be much slower. Then when I generated the .ngc file I compared it to my old one and there was only 1 line different. Everything else was identical between the two. The different line was at the top: N30 S3100 M3

In my old file it was N30 S10000 M3

So I am skeptical that this will do anything different in my LinuxCNC machine when I run it. I feel like it's still going to try to move just as fast as it was before. Am I missing something in my post processing to help preserve the proper feed and movement speeds that CAM knows I need?

Greetings,

I do not have experience with Fusion 360. However, after Googling a bit, it looks remarkably like the MasterCam software I used years back.

Check out this link...

help.autodesk.com/view/fusion360/ENU/?gu...AF-B848-8D62CAF57C49

This should answer your needs.

The difference is one runs the spindle at 3100 rpm the other at 10000rpm. Spindle speed has no direct correlation with feed speed. (unless your using G95 units/rev mode which is unlikely on a mill.)

If you only are changing the RPM that is the only change you should expect to see in the g-code. If you also wanted to change the feed rates you need to look at the F codes in the G-code file as well.

Hi Guys,

I get what you're both saying fc60 and Todd, but maybe I'm asking the question the wrong way. In Fusion 360 I see it changing the surface speed from the 300's to 100ft/min, so I know that the CAM software says to itself "OK his spindle is going slower so we now have to FEED slower" ...but that change doesn't appear to be reflected in the CAM file it generates.

So should LinuxCNC be smart enough to adjust my feedrate to now accommodate that slower spindle speed from the N30 line? -If so I should see it taking approximately 3x longer to complete an operation where it's feeding but when I time the old file against the new one, LinuxCNC runs them at exactly the same rate.

Is there something I need to do in my HAL or INI file to tell it to adjust surface speed (when feeding) based upon my spindle speed?

Spindle speed and feedrate have a correlation!

A 10 mm cutter can cut i.e. 0.016 mm/ teeth, having 4 teeth and a given Vc of 23 m/min will give you a rpm of about 800 trpm and a feed of 47 mm/min (out of memory) if you double the Vc, also feedrate and spindle rpm will grow!

So if your spindle rpm is the limit, you will need to lower the feed, otherwise the amount of material per teeth is to large and will destroy the tool!

Have you configured your tools with a feed rate or with teeth an cutdepth per teeth?

Norbert

Hi Norbert, I did change the RPM in the Fusion 360 CAM and in there it most definitely did show a new "Surface Speed". The new surface speed is how far it will travel ft/min to match the proper bite size per tooth needed.

The problem is my LinuxCNC software seems to be ignorant to this correlation. When I did timed runs without a cutting bit in the mill, it ran the program at exactly the same speed even though the new file had a different line 30. The only difference between the old file produced in F360 and the new one with the slower spindle speed was just this 1 line. OLD WAY: N30 S10000 M3 and then NEW WAY: N30 S3100 M3.

But when I ran these 2 programs in my LinuxCNC on my machine the bed moved around identical in both cases. No difference in the feed rates. So basically it would not have cared if I put 100 RPM spindle speed. The bed was trying to move just like it did before without regard to spindle speed. -Hence it would destroy my bit almost instantly.

This is what I'm asking for help with. I feel like there's some correlation between spindle speed S3100 or S10000 that isn't being observed or factored in with LinuxCNC. I feel like it's not caring what my spindle speed is and the bed is just doing its own thing.

Hi Hatch. In Fusion, if you change your spindle speed, your cutting feedrate stay's the same, but your feed per tooth will increase. You need to change your feed per tooth to the value you require, then your cutting feedrate will come down. This is a cam setting, not a linuxcnc one, as Tommy said. Hope this helps. Matt