CHECKING MINOR DIAMETER ON EXTERNAL THREAD

[Larry1958]

Im hoping someone can shed some light on an issue Im having. Im trying to do research on the proper way to check the minor diameter on a metric series M26 x 1 4h/4h 4 start thread. Im using thread check software for the specs and get "Max flat form minor diameter @24.917, Max flat width at minor Diameter @.25, Min. flat width at minor diameter @.144, Min rounded form minor diameter (ref) @24.917. The issue is how to check max minor and min. minor (or the correct way to check them). Hoping there are some Quality Control people here that could shed some light. The issue is that my minor Diameter the way we are checking it is undersize. We are checking the Bottom of the Radius at the root. I am using a standard 1.0mm full profile ISO insert to machine the thread and pitch, major diameters are fine. Thanks in Advance.

[jeff]

if you're using a full profile insert, can you just check the height of the insert and double it, then subtract from the Major?

[Larry1958]

Not sure why. I am finishing the Major Diameter before threading. Just using the full profile insert so I know i am using the correct rad., If I use a partiall profile insert the Rad. is .05 and the minor is WAY undersize (this is according to our Q.C. dept.). The problem I am having is that the customer drawing has the same information as I get from the thread check software except theres no reference () on the Minor Min. diameter callout so we are forced to hold it.

[Reko]

This is just a suggestion, it has worked for me on many threads and oddball profiles... draw the thread profile in Mastercam and then "plot" it to a transparency (mylar)... obviously you have to make sure the plotter is correctly set to scale beforehand.

 

Then, as long as you know the pitch is right, the thread form should match the mylar on an optical comparator (shadow graph).

[Larry1958]

There using a comparator to verify my Minor Dia. Min is undersize. I know I am making a good thread, passes go-no go, Major measures good, pitch meassures good over wire method and pitch mics, but the minor is being cut undersize. Everywhere I look the Minor Minimum should be a reference only, and the Minor max is the important one to be verified. Question is the way there are checking it (is it correct), Im thinking it shoud be checked at a flat form of p/4 or a flat of .25 in this case.

[Reko]

Grind the insert to the form they are asking for. You can use the toolholder to hold the insert, indicate the tool holder.

 

Problem solved.

[Larry1958]

Easier said than done. This is a production job of over 1000pcs every month.

[LaszloK]

Grind the insert to the form they are asking for. You can use the toolholder to hold the insert, indicate the tool holder.

 

Problem solved.

 

I agree that the problemm is at the root of the thread. I would draw it in MC to reduce the trial and error of modifying the insert geometry. You need to work it out on "paper" first.

[Reko]

Here are your options then...

 

1. You could call to the company that you are making the part for and ask for a variance... send them a drawing of what you can make with standard inserts.

 

2. Call in a tool supply company (several if necessary) and find the correct insert to make that thread.

 

Other than that, you will have to make a set up to custom grind the inserts... then, have a talk with whoever quoted/accepted the job without understanding what it was going to take to make a non-standard thread.

[Larry1958]

The issue is that the 1.0mm pitch is standard, and that all the numbers from the calculations are correct (thread check software). I am not so sure that the parts are being checked according to standards - in this case ASME B1.13-2005, and ISO 68-1. Follow this link http://en.wikipedia.org/wiki/ISO_metric_screw_thread You will see that the minor is being called out at the flat root width of P/4. This is why I need some Quality Control help on this. We are checking the minor at the bottom of the radius the tool is creating.

[Reko]

I could be wrong, but it seems like you are over-thinking this.

 

The minor diameter is merely for clearance. If your Major is correct, pitch is correct, and 60 degree angle is correct, I say you have a good thread... even if the minor is undersized at the bottom of the radius root... it is just clearance anyway.

 

The wiki link that you posted showed a dimension short of that... mathematically, your thread should also end up there if you inspect it at that point on the 60 degree angle.

 

The fact that your insert pushes the minor smaller should not matter... again, it is just clearance anyway.

 

For a job running 1000 pcs./month, as you say, I would also invest in thread gages (go and no/go) too.

[taperlength]

I could be wrong, but the inspector needs to back off.

[TheePres]

If these thread specs are silimar to a "J" series thread spec, the minor is definitely not just clearance as it has controlled minor diam. and root radius.

As Reko stated, find out if insert available.

[NOTW Programmer]

Easier said than done. This is a production job of over 1000pcs every month.

Have a tool manufacturer make you a tool, sumitomo can do that for sure.

[Larry1958]

This is a standard Metric series, not a "MJ". This is the problem. I have asked the Q.C. manager to please have the customer change the drawing on this and mearly state reference on the Minor Min. Diameter. He states that this is not an option and we need to make it according to print. Says that its a goverment contract and that making even as simple a change as this is a major task. Bull, I say. I've done plenty of Goverment work in the past and if explained correctly to the Engineers it has never been an issue for me. I think that they are just trying to shove there weight around personally.

[Larry1958]

ok, here's what I have figured out. 1st., we have been checking our minor diameters wrong from the start. The minor maximum needs to be checked at a flat form of p/4, this is done by measuring a line that falls parallel to centerline, at a width or p/4 till it stops in the 60 degree vee. The measurement is taken there and only to verify that the line falls below the Minor dia. maximum dimension. the minor minimum ( means nothing) but if it does need to be check it would be done at the bottom off the 60 degree vee regardless of if its a flat or a rounded form. If it is an MJ series then it is done at the bottom for both minor max, and minor min. - Now I have to convince our Q.C. dept of this. After doing my research it makes sense to verify the minor diameter maximum this way to be assured there is no mating part engagement issues. Any input? Maybe?