Ramp Angle & Plunging Approaches

[richardsalzman]

I have a few questions regarding plunging tool approaches and ramp angles.  

I used the Gwizard calculator to calculate the reduced feed rate for the ramp (see below) of 6.7 imp from the original feed rate of 8.1.  But I noted that Gwizard does not ask for the ramp angle.

My question are as follows:

1.  How do you determine the correct ramp angle?

2.  Fusion requests a max ramp stepdown (also below).  It is defined as the max stepdown per revolution.  The default value was .75 inches.  How could the tool step down 3/4" for each revolution?  

3.  Lastly, in the examples below, I could have chosen a helix ramp type since it puts the least wear on the tools.  On the arc shaped slot, I choose the "smooth profile" for the ramp as it avoids full depth cuts.  Is this simply a matter of personal preference?

Thanks.. Richard

On the examples above, I used the Gwizard calculator 

[dmealer]

I use 2deg as standard. Yes .75 inches is going to break your tool.

I usually use a .05 to .1 depending on what im doing.

Yes style is a matter of preference.

Hope this helps

[richardsalzman]

This is strange.  I just a similar part with it set at .75 and it certainly did not drop .75" per revolution.  

[DS_P · Accepted solution]

I had similar questions the other week on a part so I spent some time researching. Can't fully answer your question because I couldn't find good  "rules of thumb" on ramping but here is what I learned.

This video was helpful but didn't have as much hard numbers as i wished https://www.youtube.com/watch?v=fpJpGXAFjuY

1. If you use the ramp mini calc in GWizard (ramp button at the bottom) it lets you set ramp angle to define that feed rate.  Ramp angle is based on the end mill manufacturers recommendations. Some like the Guhring Diver series end mill can do up to 45deg (haven't used one but videos are scary looking). This is based on the available clearance in the end mill to evacuate the chip behind itself. I think pocket floor finish tends to suffer on these high ramp designs as a result.

It seems like 2-3deg is a safe bet for most generic carbide in aluminum on an industrial CNC based on readings on the internet, less for hard steels. Probably could do more.  No idea what works on hobby CNCs, wouldn't surprise me if the gantry flexing in Z caused problems or something.

2. Its not per revolution of the end mill, its per revolution of the path. If your path was long enough the angle would be the limiting factor. Or if your step down was small enough vs the path that would override angle.     Maybe .75 was a default to keep it out of the way of the angle calc? Probably just set it at an angle and let CAM do the math.

3. Helix is a constant engagement cut,  this is supposed to be nicer to endmill life (constant engagement and gives good chip evac vs a slot).   If a helix works that's my default at the moment for pockets unless someone has better advice. The taper is nice too if you have enough diameter in the pocket as it helps give room to evac chips once you get towards the bottom of the hole.

It looks like you are zig-zagging for the linear slots and doing a profile on the arc slots. Pretty much would be my choice for those, mostly personal preference/what fits the part. If I care about wall finish on the slots I might try and ramp in a slightly smaller endmill (say 10mm for a 12mm slot) then use a contour to finish the walls. If its just for a nasty bolt to pivot on I might pick an endmill to size.

Also what machine are you running and does Gwizard always feel a bit aggressive to you? I find myself using 50-70% rabbit/turtle for roughing and 20-30% for finishing. That's with all my machine hp/torque/speed definitions set and running a nice BT30 machine and good carbide.

[richardsalzman]

Thanks for the explanation of the "per revolution of the path".  That makes lots of sense.  The video is interesting, but as you noted, did not give any real guidelines.

I am running a manual mill (Precision Matthews PM833) that I converted to CNC.  This is a garage hobby for me.  I also swapped the original spindle motor for a 3.5 HP ac servo motor with a max rpm of 6000.  I also find that I dial back Gwizard quite a bit.  I really use it to get me in the range, then adjust as needed.

Having never run parts before with a fixture plate, I ran with very conservative speeds/feeds.  I didn't want to experiment on this part but I will run much faster next time.  The "profile" ramp type on the arced slot and "linear" ramp type on the straight slots worked great.  Attached is a photo of the part.

Thanks for your help... Richard

[programming2C78B]

This was posted before. The ramp angle is the main driver, but you can set a max depth as well, since that is dependent on the length of your part profile. The angle and max depth keep each other in check, and one will overrride the other when needed to maintain the smallest one. 

[richardsalzman]

Thanks!  That makes sense.  just curios, I noticed the default number for the max depth was .75 inches.  Does Fusion calculate this as a multiplier of the tool diameter?  In this example, 3 x .25 inches.

[programming2C78B · Accepted solution]

No clue, you can look at the expression on your end. I would set it to 30% tool dia for steels, 50% for aluminum and plastic. Depends on your machine and how much its engaged. 

[richardsalzman]

Thanks for your insight!

[jeffescott]

My understanding is: The maximum ramp step down is .75 in not .75 in per revolution.

The tool will ramp down at the specified angle until it is down .75 in.  You should set this value to the maximum your tool and feeds and speeds allow

[DS_P]

Last time I used zig zag ramping it was a slot path and that depth was
stepdown per zig and zag, not total depth, might function differently using
different operations.

[richardsalzman]

I played around with this a bit and I do believe it is per revolution of the path.  In a helix it would be per revolution, with the zig zag, each zig zag is in effect a revolution.

[richardsalzman]

Thanks for you help!  I used your figures for a few jobs and they work great!