[IMT]

I've never tried using Sprut to generate a thread milling tool path. I created a fairly simple macro in VB and run it as an M-Code. I hand code the parameters: Major Diameter, Minor Diameter, Depth, WOC per pass, WOC on finish pass. Then call the M code.

[mountaindew]

I've never tried using Sprut to generate a thread milling tool path. I created a fairly simple macro in VB and run it as an M-Code. I hand code the parameters: Major Diameter, Minor Diameter, Depth, WOC per pass, WOC on finish pass. Then call the M code.

Mach3 conversation wizard also has this type operation and can be performed at mill. "one hole with lots of messing around"
In my experience, sprut worked fine. just some confusion on tool definitions so simulation will show correct results.
Then setup as default parameters for half dozen thread pitches and are just a mouse click away from use.
Nice to have all those thread pitches and tapers combined with different sizes most any internal or external thread can be made.
For setup I designed a plate with different diameters and then performed different thread pitches in cam model.
Attachment 247548
Tune the settings a little
Attachment 247546
Then saved the settings for each type . Now I can do this with little effort and programing.
md

[IMT]

Looks like that works well for you. Does Sprut generate helical arcs or short line segments on this op?
How do you manage cutter diameter variation? I've found I cannot use the diameter listed on the tool but have to tweek it a little to get the thread to spec.
Does the Sprut threadmill op allow you to start at the bottom of the hole and thread upwards, climb cutting?

[mountaindew]

Looks like that works well for you. Does Sprut generate helical arcs or short line segments on this op?
How do you manage cutter diameter variation? I've found I cannot use the diameter listed on the tool but have to tweek it a little to get the thread to spec.
Does the Sprut threadmill op allow you to start at the bottom of the hole and thread upwards, climb cutting?

The operation is listed under helical machine paths under hole machine operations. The generated G-code I guess is helical not clear what you mean by line segments. "its tormach's g-code post"
Cutter diameter is measured for tool definition. The actual hole size and thread depth is what I adjust along with pitch to get the fit and finish desired.
Sprut allows both inside, outside and bottom up or top down milling along with a host of other settings you can use. I would guess many cam programs do this.

You guys/ girls that have the skill to write code, macros and other long hand or canned operations are awesome.
I have read a couple cnc programing books cover to cover and would say more then one is worthy of a 8 credit hour course in college.
As I have noted in other posts. I understand g- code but I rely on cad/cam systems to generate it.
md

md

[TurboStep]

Does Sprut generate helical arcs or short line segments on this op?

Sprut generates arcs

How do you manage cutter diameter variation? I've found I cannot use the diameter listed on the tool but have to tweek it a little to get the thread to spec.

Cutter variation? If using a thread mill with the correct form you may need to adjust the diameter to achieve the correct thread tolerance class. If you don't you'll be milling exactly to the nominal size (+/- the normal milling tolerances) which may be a little tight for some screws. Good quality screws generally fit very snugly.
If you're using a single point end mill ground with a pointed tooth you will have to calculate the effective diameter based on the threads pitch diameter. There should be no need to tweak anything - it should be possible to calculate the required thread quite accurately. This of course independent of whether you're using Sprut of hand coding.

Does the Sprut threadmill op allow you to start at the bottom of the hole and thread upwards, climb cutting?

As MD has stated, you're free to set all these parameters at will.
Step

[SCzEngrgGroup]

How do you manage cutter diameter variation? I've found I cannot use the diameter listed on the tool but have to tweek it a little to get the thread to spec.

Perhaps the confusion has to do with the difference between a threads "major diameter" and the actual diameter swept out by the threadmill when it's cutting the threads? For standard thread-forms (*NC, *NF, Metric, BS*, etc) the tips of the threads do NOT come to a point, but are rounded both at the peaks and valleys. The "major diameter" you find in all thread tables is the dimaeter of that rounded peak or valley. But the threadmill DOES cut to a point (at least in theory), so the diameter you specify in the CAM operation must be larger than the major diameter in the thread table. Sadly, the relationship between the two numbers is also quite complex, and I have yet to find a table or calculator that allows you to enter the thread spec (i.e. = M6x1 or 1/4-20) and get the correct diameter to enter into the CAM operation. I ended up creating a spreadsheet I can cut and paste the thread table data into and it calculates the correct diameter, or close to it. But, it always takes a test cut to make sure it's correct the first time I do a new thread.

Does the Sprut threadmill op allow you to start at the bottom of the hole and thread upwards, climb cutting?

In thread-milling, you ALWAYS want to climb mill, and whether you start at the top of bottom of the hole is a function of whether your're cutting internal, external, left-hand, or right-hand threads. For example cutting a right-hand internal thread, it should start at the bottom and work its way up. Cutting an internal left-hand thread, it should start at the top, and work its way down. The CAM should be smart enough to always to the right thing. I know HSMXpress and SheetCAM both are. I would assume (hope?) SprutCAM is as well.

Regards,
Ray L.

[TurboStep]

But the threadmill DOES cut to a point (at least in theory)

As I said earlier there are different types of thread mills. General purpose thread mills with single thread forms like these:
Solid Carbide Single Thread Form Thread Mills Made in USA - MariTool
will cut to a point. Others cut with the correct thread form:
Metric Thread Forms - MariTool
and therefore do not cut to a point.

Sadly, the relationship between the two numbers is also quite complex, and I have yet to find a table or calculator that allows you to enter the thread spec (i.e. = M6x1 or 1/4-20) ...

It's actually quite easy, this link explains it all:
ISO metric screw thread sizes and tolerances - Ames
(its the same for unified threads - there's also a link to the corresponding page on the right)
The key is to calculate the value of H, which they call the height of the fundamental triangle, where:
Attachment 247608
and P is the thread pitch.
if using a thread mill ground to a point simply compensate the thread diameter e.g. by adding H/8 to the diameter for internal threads.
Alternatively check the GWizard Threads tab, this shows the values for H for the selected thread.

The CAM should be smart enough to always to the right thing. I know HSMXpress and SheetCAM both are. I would assume (hope?) SprutCAM is as well.

Sprut leaves the options open. Climb milling may be preferred, but it's a free world!
Step

[SCzEngrgGroup]

It's actually quite easy, this link explains it all:
ISO metric screw thread sizes and tolerances - Ames
(its the same for unified threads - there's also a link to the corresponding page on the right)

Yeah, in theory.... Trouble is, I've rarely found this to work precisely in the real world, and I still end up having to do a test cut or two to get it really dialed in correctly. If you're making both mating parts, it works fine, but when making a part to fit something for which you don't have specs, it's hit or miss.

Regards,
Ray L.

[mountaindew]

And how I did it
I used the constants defined in cnc programing handbook by P Smid.
One of the books I referenced in above post.
These constants are referenced in chapters on both helical thread milling and single point threading on lathes.

The two common constants for calculating thread depth are 0.61343 for external and 0.54147 for internal. "book also references 0.54127" one is a typo

I used constant x pitch to calculate the major diameter and then the hole sizes for both major and minor.
I modeled the major diameter and milled the minor diameter.
Then helical milled the single point thread form to major diameter leaving sprut cam gouge detection on and letting it use modeled size.
Other settings for pitch and taper are also set as desired and g-code is generated from that. worked ok.
As Tstep mentions there are few ways to do all this.
I have made notes of the posts above and will also use these methods in future needs.
md


And a question
In thread-milling, you ALWAYS want to climb mill?
Some magic I don't understand?

[TurboStep]

And how I did it
I used the constants defined in cnc programing handbook by P Smid.
...
The two common constants for calculating thread depth are 0.61343 for external and 0.54147 for internal. "book also references 0.54127" one is a typo

Those magic numbers look really nice. Specified to sooooooo many decimal places!
The problem with magic numbers, is that if you don't know where they come from, things can go horribly wrong...... magically wrong

Checking the internet I found several references to these values but none explained the source (does Peter Smid explain it in his book?). Well 0.5414659 was quite easy to derive but 6.134347 took a couple of minutes longer!

So, for anyone who might be remotely interested...
The formula I quoted in a previous post is equivalent to H=0.866 * P. The first value, 0.54147 equates to 0.866 * 5/8. Following the link in my previous post will show a diagram of the most common thread profile. You'll see that the distance between the flats on the internal thread is equal to 5/8H. This depth is valid only for a tool with a flat at the end.
The second value, 0.61343 equates to 0.866 * (5 2/3)/8. This represents the distance between the flat crest of the external thread to the bottom of the valley shown by the radius R where the curve forms a tangent to the "fundamental triangle", and is only valid for tools with the correct radius.

Using these values with a thread mill that cuts to a point will not give you the correct thread depth.
Step

[mountaindew]

Quote from book "Cnc programing by P Smid"
Thread Depth constants!
Base on international standards. As with many constants in mathematics these two are based on main unit being 1 (one). In this case , since the thread depth will change with any pitch change, the pitch is assumed to have a value of 1. That means P=1mm or P=1 inch. There is a reason why the unit if one has been used - it allows multiplication by any actual unit value to produce the required result. The formula using such constant is usable for any pitch size. One other dimension is also important - the dimension H, overall thread height, measured between sharp points.
if pitch p = 1,
then ... h= 0.5 / tan30 = 0.866025
From the actual calculations of thread depth can be made, based on the fractional dimensions of the standard:
17/24H = 17/24 x 0.866025
= 0.708333 x 0.866025
= 0.613435 external

5/8 = 5/8 x 0.866025
= 0.625 x 0.866025
= 0.541266 internal
Hope this kind of helps explain the constants anyway.
There is complete diagrams and more math and information in the text. "much like the link above"

My understanding of threading is not complete and I pull out references like this and step thru the math and the diagrams to get numbers needed.
Then do some testing to be clear on results.
md

[SCzEngrgGroup]

The basic formulas are pretty simple. Where it gets really complex is when you start accounting for tolerances. The formulas will give you threads that, if you cut internal and external threads to exactly those numbers, they will not screw together. The internal needs to be slightly smaller, or the external slightly larger. That's where it gets tricky.

Regards,
Ray L.

[TurboStep]

17/24H = 17/24 x 0.866025

As I thought. I don't have the book, but if I understand you correctly, it would appear that these values are simply quoted without specifying a context. Obviously 17/24 is the same as (5 + 2/3) / 8, but I used this form for a very good reason - to indicate the difference between this and simply 5/8. Values like these should only be used if you know where they come from, otherwise they may lead to surprises. I suspect these values may have confused more people than they've helped. They will only work if using a cutter form designed for the selected thread.

Lets take the internal thread. The depth of the nominal thread is 5/8 H. BUT the bottom of the thread form is FLAT. If you are using a cutter ground to a point you will need to cut deeper than the flat in order to cut down to the fundamental triangle. In such a case an effective thread depth of 6/8 H will be necessary. For an external thread you will need an effective thread depth of 7/8 H (I hope I got those the right way around).

Where it gets really complex is when you start accounting for tolerances.

If you've understood what I've written above this will indeed provide the nominal thread size. As I stated in post #25 "If using a thread mill with the correct form you may need to adjust the diameter to achieve the correct thread tolerance class." The link I provided in post #27 (I only discovered this calculator a couple of days ago - I don't want to take any credit for it) allows you to select a thread type and tolerance classes for both internal and external threads. All the values that you need are calculated lower down. If using a cutter ground to a point I would select the average pitch diameter for the selected thread and tolerance class, and simply add or subtract 4/8 H.

Is this a little clearer????
This is just geometry. Get it right, and providing the tool you're using is capable of cutting the required thread, the threads WILL fit.
Step

[mountaindew]

As I thought. I don't have the book, but if I understand you correctly, it would appear that these values are simply quoted without specifying a context. Step

True
About 30 pages of context is left out in one section and another 20 pages in another section.
Sorry
As I noted above I research and follow examples to setup what I needed. "kind of brute force method"
Thanks for the link. "nice clear fast info"
md

[rlockwood]

When I cut a thread, I don't take several passes. I do it all in one pass.

Good luck with that