Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Hole Reaming Question

Message 1 of 13
368 Views, 12 Replies

Hole Reaming Question

I am using an inexpensive H7 HSS chucking reamer to ream a 14mm hole in 6061 aluminum.  The hole is 1.5 inches deep.  The end result is a cylinder for a model steam engine project (See below).  The pilot hole for will be drilled with a 17/32 HSS drill bit. 


I used GWizard to calculate the speeds and feeds of 600 rpm and 2.66 ipm to yield a smooth finish.  GWizard did not indicate a pecking depth.  When I created the tool path in Fusion, Fusion automatically defaulted to "Reaming - Feed Out" for the drilling cycle since I am using a reamer.  



1.  Do I need a pecking cycle for a chucking reamer?

2.  I have read that the feed rate for a chucking reamer should be faster than that used for the pilot hole.  I planned on first drilling a 1/4 inch pilot hole, then the larger 17/32 pilot hole.  The speeds and feeds for the 17/32 hole was calculated at 1250 rpm and 3.3 ipm with a .25 peck depth.  All feeds and speeds were calculated using the Gwizard calculator.  These figures indicate a SLOWER feed rate for the reamer than the drill.  


I welcome your thoughts with respect to verifying the correct speeds and feeds and if I need a pecking cycle for a reamer.  I am using a small 2HP benchtop mill converted to CNC.


Thanks... Richard









Message 2 of 13

No Peck with a reamer you want it Feeding In / Out like you selected, I've found GWizard speeds to be highly variable, what was your Tortise & Hare slider set approx % with 1 being 'Fine' and 100 being 'Rough'

Message 3 of 13

Thanks.  I used the most conservative GWizard setting (like 1% or 5%) since I am in no rush and want the best surface finish.

Message 4 of 13

That will definitely work and should give a good surface finish, lots of lubricant will also help


Shouldn't be an issue for the 2HP mill on the reaming side of things

Message 5 of 13

Thanks for your thoughts.  I am very new with this and really appreciate your input.

Message 6 of 13

Your problem will likely be swarf build up in the flutes, causing recutting.  I suggest slow and slow.  

For best results ream more than one or two test holes.   Make sure reamer flutes are not fully covered by remaining stock after first hole, so swarf can fall out bottom.   Down ward air blast may help

Message 7 of 13

Thanks for the nice tips.  I will go as slowly as possible.

Message 8 of 13

Is this a thru or blind hole? If it's blind, either use a reamer that pulls the chips out (A LH Spiral reamer) or allow for sufficient room beyond the reamer for chips

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 9 of 13

Thanks Seth.  The hole is a thru hole.  My concern is that the reamer I have is a straight reamer.




Message 10 of 13

Flood coolant or mist?

I wouldn't worry too much. I just wrapped up a job with a 1.001" reamer, 7.5" deep, also a thru hole. (7075 aluminum)

Slow speed, high feed is the ticket. Oh, and ample coolant if possible.

Seth Madore
Customer Advocacy Manager - Manufacturing
Message 11 of 13

Interesting.  The reason for this post was that I read that the key is a high feed rate.  I used a feeds and speeds calculator (GWizard) to calculate the speeds and feeds of 600 rpm and 2.66 ipm to yield a smooth finish.   The pilot hole is 17/32.  The reamer is 14mm so there is not a lot of material being removed.  I am using a H7 HSS 5 flute chucking reamer (not a high end reamer) with mist coolant (Fogbuster).   The reamer is a straight flute reamer.


2.66 ipm does not seem like a high feed rate.  What would you recommend?


Thanks... Richard

Message 12 of 13

The GWizard entire range from Rough (100%) to Finish (1%) for a 14mm reamer is


100SFM @ .0089 IPR

90SFM @ .0044 IPR


17/32 to 14mm is about .020" of material removal, which is midrange between the recommended .011" to .028" undersized hole


the Machinist Handbook page on reaming difficulties says .0002" to .0005" feed per tooth which is in line with your speed / feed on a presumably 6 or 8 flute reamer



 Somewhere in there is 'your' answer to your situation but you need to try it and adjust, you have pretty good starting parameters I feel


The feed is mostly to address chip buildup in the hole, and flushing + leaving less material to cut will help, but there are limits


You're about in the middle of these ranges which to me is a green light

Message 13 of 13

WOW.  What would I do without this forum.  Thanks for all the insight... exactly what I was looking for.  Kind of funny.  I just ordered a copy of the Machinist Handbook a few days ago and while waiting for it to arrive, I was wondering if it addressed this topic.  Thank!

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums