Compensating feed rates on arcs

[Hugh.Venables]

When a cutter is moving through an arc in a cylindrical pocket if the specified feed rate presumably applies to the centre of the cutter then the cutter teeth will actually be feeding at a greater rate. This will become increasingly significant as the arc gets smaller in proportion to the cutter diameter. Can MC compensate for this?

Hugh Venables.

[Kenneth Potter]

Job setup

Look at

Adjust feed rate on arc move in the feed rate calculation area. Set your minimum feed rate there. Also try using the high speed machining option. There you can set up custom machine setting with lots of options to get what you want.

Hope this helps

[Hugh.Venables]

Thanks Kenneth.

Maybe I need to open my eyes a bit wider. It works well. Because it is set in Job Setup it is applied to all operations, not always desired. In that case it might be better to try High Speed Machining to be able to tailor that one operation. Sometimes the surface machining tool paths produce files that our control can't process fast enough to keep the machine running.

[Kenneth Potter]

In the HSM function can set up your accelerator & decelerator feed rates. you can also save your custom settings as a machine file type. Lots of tools inside the HSM options.

Kenneth Potter

[Hugh.Venables]

Actually "adjust fee on arc moves" in Job Setup seems to grossly overcompensate. I believe the compensation factor is 1-C/J where C is cutter dia and J is job arc dia. I'm doing a job where I calculate the feed needs to reduce from 60 m.m./min (2.36 IPM) to 2.3 (0.92 IPM). One third the way down the profile MC has already reduced it to 0.1 (0.004). Any ideas? Can anyone confirm my formula?

Hugh Venables

[Consultant]

The best tool for feedrate adjustment, that follows the physics of the machine and utilizes that information is Metacut.

This will optimize your toolpaths, fit arcs if you havent done so with Mastercam filter and insert the appropriate arc feedrates.

They have been in this business for 8+ years and are the best.

Check them out at www.metacut.com

 

Regards

[Glenn Bouman]

MetaCut will change the feed of a arc based on its radius to compensate for the limitations of the machine not on whether it is an inside or outside arc like Hugh was asking. I do not know what formula job setup uses.

[Consultant]

The logic is the same. Job Setup uses a calculation that is a lot simpler than that of Metacut.

Besides, what is the difference when you are cutting inside a pocket (arc's with smaller radii) or cutting outside the pocket (arc's with larger radii). I am using pocketing as an example to illustrate the point. So, you naturally need to minimize the feedrate on a smaller arc and maximize on a larger arc(both to the capabilities of the machine).

Then again, are you talking about roughing operations or finish operations?

Mastercam's arc feedrate adjustment tool that is available via the Job Setup or via the individual toolpath operations is decent, but not as detailed as the Metacut software.

Mastercam's Highfeed tool is pretty good for what it does. There are however limitations in this tool where the acceleration and decelaration are based on studying the optimal machining feedrate of 1 arc. Also, the cornering feedrate is based purely at 90 degrees. Other angles at which the tool can accelerate or decelarate are not taken into consideration. But, for being included in Mastercam, it is an excellent bargain!

I hope this has not gone off track from the main point of discussion, but all the above points do matter.

Regards

[Consultant]

Mastercam's method of calculating arc feedrate adjustment is very basic and does not take into consideration a lot of variables that are required to calculate the optimal feedrate for the arcs.

For a good comparison, the best tool as I suggested before is to try the Metacut software and do a comparison of how they both work. I am sure you can do a 30 day trial of the software. This will probably give you a better idea of how the other software works and how Mastercam's works.

At the least, if you dont want to buy anything, you get a better understanding of their logic.

Regards

[Hugh.Venables]

Thanks Guys. I've just downloaded the 30 day trial. I'll see what it can do.

Hugh

[Glenn Bouman]

The differance between cutting an inside arc and an outside arc has to do with chip thinning

http://www.otmtools.com/tech_milling.htm

Mastercam's Highfeed will fix the problem.

[Hugh.Venables]

Glenn, thanks for your further info. I had a look at the site but didn't see any mention of feed compensation on arc moves.

From purely a geometric point of view, if a cutter is making a light cut around the inside of a radius, the feed rate as applied to the centre of the cutter has to be slowed down if the feed per tooth is to be as intended. As the radius of the cutter approaches the radius of the job, the feed rate approaches zero.

If the cutter is cutting around the outside of the radius the feed rate needs to be increased to preserve the intended FPT. For example, if a 5/8" cutter is cutting a 0.035" radius the feed rate needs to be increased 10 times to get the same FPT as cutting in a straight line.

Hugh.