Lathe Threading Tools no SFM option

[thuren.machine]

Hello,

As the title says, I am threading an OD bar and I am trying to output my lathe threading tool with SFM rather than a set spindle RPM and I cannot find anywhere to change the option in my cycle from RPM tp SFM. I have looked through the tool definition as well as through all tabs in the threading toolpath dialog. Thanks for any help.

[seth.madore]

They removed the option for constant surface footage several months back. Why? Real world application proves that CSS with threading will often result in poor quality threads

 

[ChrisDPCnc]

Flabbergasted!

95% of everything we make has a thread and we use surface speed to calculate the RPM every time, making different threads at different diameters in different materials will require different RPMs to make quality threads.

Real world fact.😁

Did the Fusion team call in threading tool insert manufacturers for their take on it?  

All the data provided by the likes of Sandvik, Seco, Iscar is in Surface speed....

[Anonymous]

Using appropriate surface speed for material in question is not being contested by any means, you definitely want to distinguish between Inconel 718 and brass by calculating surface speed for given diameter and material but once you have the figure, that figure should be used as constant (G97) speed for threading.

If you were to use G96, your effective range for speed change would only apply to difference between minor and mayor diameter, however, because tool has to retract above or below threads to clear, machine would have to adjust speed in range from current cut to retract diameter.

That speed change would dramatically increase and decrease in value in every pass as you work with range of diameters.

In such high pace speed change, tool would have to wait for speed to stabilize before starting next pass. some machines have to use dwell to insure that tool waits for speed to adjust.

This will needlessly stress drive belts, promoting premature wear, encoder needs to keep track of every pass or you will have variable pitch on front threads or worse, like cross threading.

Desired and theoretical speed may not be possible if you want to avoid chatter on last few passes as tool becomes engaged with full profile and therefore selecting "real world" speed in threading is dependent on factors such as type and depth of thread, tool properties, rigidity of tool and workpiece, material type, coolant type, required form precision and surface finish, tool life .. etc.

Rough example, without looking up actual thread spec's, clearing each pass by .1 on diameter

If I want to cut 1."- 12 external threads on 304 SS and assume surface speed of 300 FPM than, (300 * 3.82) / 1.1 = 1041 RPM

Subtract 2 times depth of thread and I get approximately .91 diameter, my speed for tool minor diameter of thread is  1259.

If I were to use G96 S300, spindle speed would be fluctuating between those two values, adjusting incrementally for every pass.

If you now consider 1/2" thread at same surface speed, values dramatically change and that is just not how it works in real world.

I can consider correct surface speed for material and diameter in question, but final value goes in G97 S??? and will be determined by combination of other factors, in most cases spindle speed will be compromising factor to meet other requirements and priorities.

While using G96 makes world of difference in facing off stock or profiling large part, adjusting difference in spindle speed between minor or major thread diameter and retract clearance does not have any measurable benefit in threading.

If I ever had G96 in threading cycle, it was by mistake and it never produced any benefit wordy of mentioning.

I am open to learning new tricks but some things just don't qualify after many years of proven methods and thousands of parts done using techniques that work.

[thuren.machine]

Oh, this is news to me! Do you have an article that gives a more thorough explanation of this idea? I did a brief search and did not find any good information on it. With the advanced machines of today, I am not sold that using CSS will affect the synchronization of the spindle and feed cycle. When your thread depth is only 0.01-0.05" deep, your CSS doesn't require a large range of adjustment compared to say a facing cycle where your theoretical center becomes null. I guess I am just not sold on the fact that RPM is superior to CSS in a lathe threading cycle. It would be nice to have the option to go either way.

[thuren.machine]

Could some spindle change cause wear on the machine? Absolutely, but the spindle changes constantly on a lathe and I would say this is a very weak point to argue against using CSS to cut threads. If your retract is only .02" above your part, your spindle change is very minimal and the dwell times to synchronize your RPM and feed are equally minimal. 

If using a set RPM is superior, it would be nice if the CAM system could identify your major diameter in the manufacturing environment, while the user inputs their desired SFM and the outputted RPM is a calculated RPM as a G97. Could the user calculate this on their own for each instance? Yes, but it is defeating the purpose of using this very powerful technology to avoid mistakes when the user is doing their own calculations outside of the software.

[Anonymous]

For Fusion to consider calculating or rather estimating proper spindle speed, you will have to provide more then diameter of stock and type of material, in contrast you can just enter value after considering all the factors at hand and deciding on speed that is likely to be good choice.

I disagree with any arguments in favor of using G96 in threading cycle because potential benefit in speed adjustment between diameters determined by depth of thread and however small retract value you like to use, is insignificant factor in larger scheme of things I explained above, you are more likely to cause problems then solve any.

Retracting only .02 from threads is inadequate clearance, chips can get trapped between tip of insert and threads, time saved by avoiding adequate retract is going to be in nanoseconds, while promoting potential problems.

If you also start threads too close to part face to save time, high pace of spindle speed fluctuation will in fact do more damage then good to equipment and threads accuracy.

With difficult materials, I often used one tool to rough threads and another to finish last few passes.

In that scenario, precise distance of both tools from part face is critical in avoiding cross threading and so is constant spindle speed. 

If this is a case of, "I want something and it's not there" or "Give people what they want", ..... question comes up, do 100000 people have to disable something on daily bases so that 10 people can have convenience of having it their way?....  or does software have to follow some common sense in providing global benefit to majority of users?

Maybe Fusion needs to provide more robust way to personalize the software and let everyone live their philosophy on their own terms for better or worse, wouldn't bother me a bit but I try to provide valid arguments in favor or against anything if I have any knowledge on subject, which I think I do.

[thuren.machine]

After all this talk of precision and how important it is to maintain spindle speed and feed synchronization, you're going to throw in a tool change and introduce some new error?  What if your roughing insert has the slightest difference (0.0002") from the finishing one? You're back-tracking on previous points you made regarding precision and the introduction of error due to using CSS.

As mentioned above by another user, all reputable tooling companies put out their speeds and feeds in terms of SFM. This isn't a "I want it my way" statement. It is a "every reputable tool company does it like this so why doesn't Fusion?" statement.

I'm still not sold on G97 vs G96 in lathe threading and machine wear is not a good point as the machine is constantly wearing so long as it's making chips. Please share some articles regarding this because I am legitimately interested in reading the facts about it.

[Anonymous]

In 32 years of doing lathe work, you are the first one to invest such time and effort to try and convince me that what I am doing is wrong.

I did in fact use two tools to do threads, leaving approximately .005 for second tool,. not .0002, I push limits where possible and beneficial, change rougher and preserve finisher.

There was never argument against use of correct surface speed, the argument is against changing range of speed within depth of thread which invites problems and yields nothing of value.

As far as reputable tool companies go, their data on back of insert box is not obtained under variety of conditions we encounter on daily bases, they test in near ideal conditions to beat or at least claim they beat the competition so take anything coming from that source with dose of suspicion. 

It took over a year for CSS default to be taken out of threading operation and now you are saying, put it back without providing any reasonable argument in favor of it, sorry but opinion does not count as reasonable argument.

[Anonymous]

I'll give you one solid argument for keeping spindle speed constant in threading.

If you use G96 to adjust speed at each pass on external thread, speed will increase with every pass.

As tool takes decreased depth of cut and speed increases, there is a good chance that it may work just fine up until very last pass when full profile of insert forms final thread profile.

So now you have chatter that can no longer be undone, part is ruined and that could have been prevented by keeping spindle speed constant, surface speed calculated for pitch line of threads.

This scenario would benefit your case in internal threads as spindle would be slowing down with each pass and somewhat be in sink with decreased tool load as a result of decreased depth of cut.

I have not even mentioned geometry of cutting edge, depth of thread, material, thread profile type and so on,..... just increase of spindle speed by small value that happens to be over the threshold for combined conditions and part gets wasted,  there is no problem with small slug, just fix the problem and make another one,..... but that doesn't work like that with large and expensive parts.

Hope you see the difference between theory and practice without having to learn the hard way. 

[seth.madore]

I would add a couple notes;
1) I made the mistake on my Doosan lathe of using CSS when I first got it. My threads were HORRIBLE. These were just a 3/8-16 UNC for a fixture, but when I went to a fixed speed, they were beautiful.

2) There was never an SFM field for threads, just Constant Surface Footage. I've started a discussion with the turning developers to consider adding a SFM field. This "may" be a Tool Library team question, so the answer may not come back until next week

[Anonymous]

Take a look at this article for some clues:

https://www.thomasnet.com/articles/machinery-tools-supplies/thread-cutting-on-lathes/

In high speed threading, if you use G96, spindle speed is adjusting up and down twice in single loop.

If spindle drive belts are not properly tightened they will slip due to frequent and abrupt speed change, bad news for point of entry on next threading pass.

Mastercam has choice of both types of speed, it assumes user knows what he or she is doing and if not, there is learning curve and damage report along the way.

I actually like that approach, let people express themselves,..... at their own expense.

[ChrisDPCnc]

That all went deeper than the point I thought, in my head, I was trying to make😃

I was just hoping to have the option of inputting Surface Speed data and having Fusion do the maths to calculate a suitable RPM value based on the thread diameter for me.  We always thread in RPM, lathes would have a hard time syncing Z moves against spindle rotational position otherwise. 

This is just what I'm used to seeing in other software, AD and other brands, and makes just makes programming one sum quicker. 

[Anonymous]

Somewhere back there in my posts I made a distinction between running threads in G96 mode and having Fusion calculate proper surface speed for running with G97.

The reason for "all that" is that OP insisted on running threads in G96 mode and experience says otherwise.

So let's look at the possibility of having Fusion suggest proper speed, you enter major diameter and......  boom, there is your calculated speed, right !?

What about the rest ?, like:

OD or ID, square shank or boring bar,  if threading bar - length from holder, material type, stock overhang from chuck, type of thread, acme, buttress ...., thread depth, cutting technique, insert cutting edge profile - flat, positive or negative rake?, ground or molded cutting edge?, barstock or single piece material, coolant type, risk factor in scrapping part if speed causes chatter, precision / size of thread profile, tool life, cycle time, length of threads, machine in question and its ability to comply,.......... did I miss anything?😋

OK, so AD will have to engineer a survey, you enter the survey and answer all these questions,......... then at the end Fusion evaluates all the data based on preloaded logic and produces compromising RPM value that hopefully satisfies all conditions for best outcome and if that doesn't work you come back to this forum and scream bloody murder because "Fusion" caused you to scrap part,......... or pick up a calculator, get your number and take a good look at all your cutting condition, make educated guess and give it a try, if it works don't mess with it and if it doesn't adjust as you see fit.

Is it overkill or do we now have more clear vision of why things are done the way they are done and why questioning that is not a good idea?😁

[Anonymous]

I need to add few more comments here for someone not as familiar with concept of single point threading to gain full picture .

In any discussion of technical nature it is often assumed that participants are aware of basic concept, that however is often a mistake and some things need to be spelled out.

Since I never run threads in G96 mode, I don't have problems associated with change of spindle speed.

So what is the problem other than those mentioned before ???🙄

Well, encoder needs constant spindle speed to track start point of thread and prevent cross threading between multiple passes.

It is entirely possible that you may not see any ill effect on 48 TPI threads due to very small difference between major and minor diameter which in turn keep speed change to values that do not result in cross threading.

If you now try that with 8 TPI, there will be significant difference in speed change from first to last pass due to difference in major and minor diameters plus the retract distance.

I deburr threads in machine 99% of the time and that involves rerunning turning tool over front chamfer and major diameter if not using full profile threading insert, and rerunning grooving tool over shoulder undercut chamfer if present, then rerunning threads to roll small burr out of threads.

In doing so I repeat last pass as a spring pass or take final cut up to .0005 deep depending on material.

So here is the point, tool reentering finished thread must start from exact same distance from face and spindle speed must be the same as one used to cut threads first time.

If you change spindle speed and attempt to rethread, result will be that tool will have different start point, it will cross thread existing thread, blow insert tip due to misalignment and scrap the part.

Value by which spindle speed is changed, up or down, will determine margin of misalignment and damage.  

[thuren.machine]

Thanks for starting the discussion, Seth. What I am imagining is that when you choose the threading option, the first tab for the the threading toolpath would have inputs laid out something like:

Basic Major:

Thread Pitch:

SFM:

And from there RPM would be calculated? Simple and effective with basically all required information in 1 place for easy calculations.

[Anonymous]

After all that I think we can at least aggrege on two things:

1 - We aggrege to disagree

2 - Bold people can't have bad hair day 🤣

[thuren.machine]

1 - If looking for a study that compares 2 things with actual data is a disagreement, then yes we disagree. I am simply for the best solution and I often play the devils advocate when debating a topic. The blanket argument of "this is how we've always done things" has never sat well with me as I have seen the technology advance exponentially in my time as a machinist and have seen that statement blown out of the water time and time again by more progressive machinists.

2- I think the saying you're looking for is bald people never have a bad hair day?

I will definitely say that I am happy that this discussion has brought some attention to the topic in an effort to streamline how threading speeds and feeds are calculated within Fusion. 

[Anonymous]

Progressive is always good thing, if it doesn't progress in wrong direction, some things are set in stone for a reason but if your wish gets honored in next update nothing goes in or out of my pocket as a result.

Fusion should weigh that request or wish with consideration to facts as noted earlier.

Giving you basic surface speed without considering numerous factors governing how that speed is determined is going to effect those who have full faith in Fusion to produce results they have yet to understand in their own experience.

My crystal ball indicates cloudy future in threading if software is tailored to suggest speed derived from diameter alone, that will scrap parts and crash tools when user has no adequate knowledge to make better judgement.

Any change that takes things in opposite direction of logic, is just another obstacle to overcome by those who know better. 

I don't think Fusion should be catering to users requests in many cases because there are standards that should not be influenced by opinions. 

Also, I have very little hair left, no bad hair days here, in part because I never needed Fusion to tell me how to produce threading cycle that works as I intended. 😁

[daniel.pacific]

FYI to this thread, on Page 26 of the Fanuc operations manual

*Because the constant surface speed control is effective during scroll thread or
tapered screw cutting and the spindle speed changes, the correct thread lead
may not be cut. Therefore, do not use the constant surface speed control during
threading. Instead, use G97

Basically, threading requires perfect synchronization between spindle revolution and Z-axis motion to allow precise chasing of threads. Constant surface speed will basically start to chip your threads with overlaps due to the acceleration/deceleration timing. 

I believe you can set SFM via a post-out option but in the dialogue it's only asking for RPM. But the calculation for SFM is in there or at least can be spit out after the calculations. It's just RPM * Diameter * π/12 = SFM