Drill and tap operation


Just ordered my nomad and had a question which I thought some of you might know the answer to.

Can the nomad support drilling and tapping operation?

I will be making some parts that require 2mm blind holes into t6061 aluminum with associated m2 tap.

Is this possible?

A friend said “tapping requires a fixed ratio of rotating speed and feed rate”. This led me to think this is a software thing and not a cnc machine thing. I could be wrong.

I remember reading on the forum that meshcam does support drilling now however wanted users and people in the know to comment.

Thanks in advance!

Yes, one can use a threading tool to cut inside or outside threads.

Video here:

Possible software tools:


In the video @WillAdams posted they are cutting M3 threads. The M2 threads you want to cut seemed really small, but after a quick search it appears that Harvey Tool makes metric thread mills down to M1.6:

1 Like

Fusion 360, a very popular software among members here has the ability to drill and create threads.

1 Like

Drill and tap - yes, but . a little different than you are thinking - it’s thread MILLING, not thread cutting, as you would with a tap…it’s not tapping. Will and others are refering to using a threadmill to cut threads, which does not require the fixed ratio of speed to feed rate.

1 Like

Do note that threading on the Nomad is done with a thread mill (see the video linked by @WillAdams ), not a tap like when cutting threads by hand.

2mm screw requires a hole that is less than 2mm (for M2-0.4, the drill size is 1.6mm), and is in the practical range for the Nomad, in my experience. Drilling takes a lot of torque, so larger holes (the exact size drilling becomes impractical depends on the material, drill type, and the drilling strategy) are best milled as a pocket.

Thread milling is pretty fast and efficient, and allows for fine tuning the thread fit, but the tools are more expensive than taps (not wildly so) and there are concerns to avoid tool breakage (depth of cut, feed, speed, and chip removal come to mind. THe work is in tight quarters)


thanks so much for the info guys! greatly appreciated ; )


Hi Fellas, so on the phone with Harvey tools and it appears that the M2 thread mills have a shank diameter of 3mm however when converting the 1/8" collet size to metric, it is 3.175mm. The concern is the collet not gripping the mill enough. What is the experience of the group? will the collet grip enough?

The ER-style collets in the Nomad have a wider clamping range than other collet styles — that said, they’re available in a variety of diameters, so I’d recommend getting 3mm collets from a reputable supplier.


For threading, you will need very low runoff so it would be best to get a 3mm collet so the bit sits properly in the collet.

1 Like

wow, super fast replies- thanks. Sorry for the super noob questions but I’m coming from 3D printing the learning curve is steep but the Nomad design, features and supporting software are making the transition easy, not to mention the member support : )

So, now to the dumb question. For the spindle on the nomad, how do I know what collet is compatible, meaning do I just search 3mm collet? assuming it would sized ERxxxx where xxxx is the number I’m looking for.

All ER11 collets will fit in the Nomad. There are other ER sizes which won’t fit. MariTool sells good quality ones for a reasonable price. Might also be a good idea to pick up a collet nut so changing tools is a little easier.


I will ask where you are located, as, if you are outside the US, you may have different sourcing options, and in some places in the US, you may have local sources that are more economical than others.

As an introduction to ER collets, you might want to look at the Haas video “ER Collet Essentials” on youtube. (search “HAAS ER COLLET ESSENTIALS” on google or search engine of choice it will be near the top)

If you invest in the 3mm collet, be aware that ER collets (in ANY series) can not be used for larger than nominal, not even 0.01mm. Be careful to keep track of which is which. I don’t know that it is really needed. These collets run quite true within the entire closure range, hold well across the entire closure range, and 0.17mm (1/8" collet on 3mm) is well within the rating, but you might get slightly better results with the 3mm.

With a small thread mill, I would be more concerned about runout due clocking the tool and collet in the holder than due to collet size. If you have available, use a 0.0001" or 0.002mm test indicator on the tool shank just above the business end, and rotate the spindle to measure runout after snugging. If it is more than you want, loosen and resnug. Also try rotating the tool and collet in the spindle then resnug it. You will likely find small variations due to position, and small variations each time you snug in a given position. This is normal, and you just find acceptable runout and go with it.

When using the thread mill, you will need to compensate for the exact size. If you can test the threads with a go/nogo gage, that is best, but for many purposes, is not needed. Start by specifying the tool as LARGER than it really is in the CAM-- a few 0.01mm–, especially if you have only catalog tolerance (not the exact size), so the cut will leave a little extra material, then run a thread and check. Adjust the size of the tool smaller in small increments until you have it correct. It is common to sneak up on proper size, especially for critical dimensions and very small features. It is also common to tweak the tool size as needed to tune a fit or adjust for actual tool size variation (new, the tools from reputable suppliers used in these machines are usually pretty tight on tolerance, but it doesn’t hurt to check. Resharpened can vary a lot)

1 Like

Just two cents here; definitely agree on milling the holes over drilling, spindle torque becomes a problem, e.g. I was not able to drill 1/8" holes in aluminum with the Nomad, probably unsurprisingly, but had zero difficulty spiral milling it.

As far as the thread milling goes, it’s definitely cool to see a threadmilling operation in action and even cooler when it actually makes a threadform you want! In the times I’ve needed threads, I have tapped by hand off the machine. Might be more manual work but it does have some advantages; eliminates(??) programming risk for threadmilling, removes risk of thread mill running out of room at bottom of blind hole due to chip buildup and tapping debate-ably is more likely to make the correct form.

If you are machining a fixture in place however, you might have no choice but to get out the threadmill! Although what you really want to use is a ‘thrill’, a super ill-advised combination drill + threading tool…they actually do exist :wink:

1 Like

Thanks again fellas. I’m located in Toronto Canada however have friends in Michigan I see pretty often. I believe there are local options so need to explore that too.

Love the advice, greatly appreciated! I was on the phone with Harvey Tools for around 40 minutes as we went through options. So, lots to think about it before I pull the trigger on these bits.

1 Like

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.