[KSky]

I have to make a large number of threaded holes in an aluminum plate and wanted some advice for those of you who have been there as I don't want to break any of these $75 mills. I am running BobCad V27.

I ordered one of these "1/4-20 Variable Flute Carbide Thread Mill" from LakeShore Carbide.

The video's from BobCAD that I found use a single profile thread mill, any video's/tutorials with V27 using a variable flute? Is the programming the same for a variable flute one?

There really isn't any starting from the bottom with a variable flute one. Is this likely to get gummed up with aluminum?

[jrmach]

I would imagine it would be treated as a multi-flute.

I never used one of those.I would say call the company,,here is their number

[KSky]

Lakeshore provides information on how to code your own routines, but they are not able to tell you how to do it in BobCAD, for that I need BobCAD. I will try opening a support case with them.

[jrmach]

Well,your not understanding.
In the box that says threads per revolution,,what that means is how many threads will your tool cut with a revolution.
Say it was not variable pitch and it had 8 rows of teeth (counting from the bottom,counting vertical to the top.,,,you would enter 8.
Remember,you are not counting flutes,you are counting rows of teeth.
The variable pitch I imagine it is the same way,but there will be teeth missing in each row.I don't think that will matter.I think you are just concerned of how many rows of teeth there are.

[KSky]

OK, that makes a lot more sense to me.

I tried creating a simple part with five holes to thread and the resulting code looks pretty good, but the simulation gets an error. Is there another obvious thing I am missing.

[jrmach]

I would suggest a search of the "help" files and a search on this forum to really get a grasp on this.There have been discussions on this before going into a little more detail.
I would share a file,but I am on Demo with V27.
I included a screen shot with the correct data entered.
Also you need to change your lead in and lead out to a much smaller number or you will gouge.
Also make sure you set your speeds and feeds a realistic value.
Off the Computer for tonight,if you need more questions answered,maybe someone else can help.
BTW,the Professor Video's Series covers this well.But that costs money..........

[JVH58]

I have a simple fix for you as far as the error message your getting. See attached image. You need to FIX the "Thread Height" value in the "Parameters" tab. I see jrmach has also shown this change.

[KSky]

That fixed it up, thanks.

Now for a feeds and speeds question. Instead of lowering the feedrate, I generally take thinner cuts but this is thread milling. Is that done with the thread diameter and have multiple features?

This is a 1/4 x 20 thread in aluminum. Per the Lakeshore carbide chart, the proper feedrate is .0015 to .0025 inches per tooth.

http://www.lakeshorecarbide.com/pdf/...mendations.pdf

[jrmach]

I never have used that kind of thread mill.
If it was me,I would follow what Lake Shore Carbide suggests,,,They are a highly regarded company.

If you were doing some nasty metals like 304,316,inconel,etc.,,,Then that could very well be a good strategy.

I just looked at their charts.Notice the feed per tooth is pretty close on all metals ?
That tells me they are concerned with chips loading the cutter.
The speeds vary a lot ,which makes sense.
So,to me,,they are taking in account for chips to excavate and not re-machine them.
Unless you are having issues with burrs or holding tolerance,,I would stick to what they suggest ???

[KSky]

That's one of the things they told me about with their other cutters, use an air blast to make sure chips get cleared out.

Back to my question, how do I take multiple shallower cuts with BobCad and the thread milling strategy?

[jrmach]

Well,if your wanting to do it I would do it with 2 features.1st feature 2/3depth of thread,last feature full depth.
I take it you don't have FLOOD coolant ?

[KSky]

Well,if your wanting to do it I would do it with 2 features.1st feature 2/3depth of thread,last feature full depth.
I take it you don't have FLOOD coolant ?

I have a Tormach, so yes, flood coolant. Sorry for all the questions, I just don't want to break a $50 thread mill on my first shot.

[A1CNC]

There are a couple ways to do multi-pass. You could change the tool diameter setting in the set-up dialog or you could change the thread diameter in the set-up dialog.

You would have to do multiple features though.

I have used that kind of thread-mill before.

I usually run them in one pass in aluminum, hell even in 303 ss as long as you get the feeds right.

If you are really concerned about breaking it, just rum it at ~40-50% of recommended to start. You can go faster later but you can't re-do it if you broke it!

[KSky]

So do these setting look pretty good for a conservative (I don't want to add to my already too large carbide scrap pile) start?

It's going for one cut (thus the diameter of .25), but slowly.

[handlewanker]

Hi, pardon me if I ask a simple question as I'm quite new to the CNC scene , but learning fast......does the thread mill cutter have multiple grooves around it's diam with no helix and at the pitch required?

This then would enable you to cut any thread with the same pitch irrespective of the diam etc?

If that is the case do you enter the tool full depth down into the hole and cut into the side wall of the hole and produce the thread helix with one turn of the XY move as the z axis goes upwards for one pitch distance?

In other words, one turn of the XY interpolated circle along with the Z axis movement produces the pitch for all of the threads simultaneously........can that be for right or left hand threads too depending on if the Z axis moves up or down?

So.......if you have a hole and make it bigger by using the XY moves and at the same time apply a progressive Z axis move at a pitch rate...... you get a thread?

That seems so easy and simple......I always assumed thread milling was done with a single point tool, like a boring bar, and cut the helix from bottom to top in a number of passes like you'd do in the lathe by having the spindle synchronised with the XY and Z movements.

Instead of a multi groove cutter could you use a single point tool, still rotating like the thread mill (much cheaper and easy to make a single point tool by hand) and after the first XY move is completed with one helical groove produced just continue on doing the XY move and the additional Z axis one too until you get to the top of the hole?

If that is the case, would thread milling just be a G code procedure?
Ian.

[A1CNC]

KSky,

Those settings should work for you. I frequently use .0005"/ tooth feed.

It seems slow but it's waaay faster than trying to remove a broken tap!

Handlewanker,
Looks like you have a pretty good idea now about the threadmilling procedure. and yes it becomes a g-code procedure. Some of the threadmill manufacturers offer free g-code generating tools on there web-sites

[handlewanker]

Hi, thanks a million for that.......made my day........I'm beginning to see the wood from the trees.....LOL.......the learning curve is flattening out a bit.
Ian.

[enauman]

I have been using BobCAD for 8 or so years and have done a lot of thread milling. I use a single thread carbide cutter because you can do multiple thread pitches with one tool. I have 2 cutters. A 0.25" dia and a 0.5" dia. When I first started to cut threads, (when cutting something like 304 stainless) I cut the depth in 3 passes by varying the tool diameter. But I have since found that I can cut most threads up to .060" deep in one pass safely by adjusting the feeds and speeds conservatively. I have cut threads on large (8") and small diameters (5/16") with no problem . I have yet to break a cutter.

As a side note, one thing I found out regarding thread depth is that the cutters I have only have a small radius in the end So I have to adjust the thread depth to something just shy of a sharp V thread. Otherwise the threads are not deep enough. I thought it would be nice to have a cutter with a flat on the end so it would cut the the right depth but then I would essentially need an cutter for each thread pitch because the flats are proportionate to the pitch.

[enauman]

The variable flute is no different programming-wise than a straight flute thread mill. You need to set the threads per revolution parameter in BobCAD to reflect the number of threads your cutter can make in a single revolution.