Help with Machining

Help with Machining / Threading / Tapping

I need to manufacture a component from Mild Steel Bright Bars. I've enclosed the drawing herewith. While the machining tolerances are pretty wide the main criteria is roundness (on OD & ID) with reference to the thread.





Current process is

1) Cutting on Bandsaw
2) Drilling required hole on conventional machines
3) Machining ID 21mm, Small Face & Champher on CNC Lathe using a Hydraulic 3 Jaw Chuck
4) Machining rest of the area along with thread using a Tap on a CNC Lathe using Expanding Mandrel to Clamp the bore machined in previous setup.

While there is almost no ovality on ID or OD when checked on a mechanical comparator. When I check it after fastening it on a screw it shows random ovality of 0.1 to 0.25mm where as the acceptable tolerance is 0.15mm.

Please guide me what to do to get the component in required tolerance.

Are you refering to runout?
I'd bore and singlepoint the thread. A drill and tap could walk.
Standard practice here is any callout related to threaded holes is measured off the minor dia.
I don't think I'd screw it on a bolt or thread gage and expect any accurate runout readings.
There's slop between the mating threads.

PS: you might want to change the topic title.

Prasham said:

I need to manufacture a component from Mild Steel Bright Bars. I've enclosed the drawing herewith. While the machining tolerances are pretty wide the main criteria is roundness (on OD & ID) with reference to the thread.


View attachment 176008




Current process is

1) Cutting on Bandsaw
2) Drilling required hole on conventional machines
3) Machining ID 21mm, Small Face & Champher on CNC Lathe using a Hydraulic 3 Jaw Chuck
4) Machining rest of the area along with thread using a Tap on a CNC Lathe using Expanding Mandrel to Clamp the bore machined in previous setup.

While there is almost no ovality on ID or OD when checked on a mechanical comparator. When I check it after fastening it on a screw it shows random ovality of 0.1 to 0.25mm where as the acceptable tolerance is 0.15mm.

Please guide me what to do to get the component in required tolerance.

Click to expand...

first off a mechanical comparator is an indicator...YES?
secondly like someone said above you cannot check it screwed on a thread since there is a .005 clearance between the roots as you know.....so what you do is this...get apiece of aluminum or brass....turn the required threads and use thread wires and the machinist handbook of the correct dimensions so you make your guage EXACTLY in the middle of tolerances (5H 6H or whatever)...make sure you use a center drill at 1st operation to insure tap straight...single point them just a few passes and leave a little stock....now run the tap in and it will follow the perfect threads you have roughed in...then use the gauge to make sure they work good and in tolerances...WALLA

PS...I assume those threads are 6H/6H....here read this



Thread Tolerancing

A full designation for a metric thread includes information not only on the thread diameter and pitch but also a designation for the thread tolerance class. For example a thread designated as M12 x 1 - 5g6g indicates that the thread has a nominal diameter of 12mm and a pitch of 1mm. The 5g indicates the tolerance class for the pitch diameter and 6g is the tolerance class for the major diameter.

A fit between threaded parts is indicated by the nut thread tolerance designation followed by the bolt thread tolerance designation separated by a slash. For example: M12 x 1 - 6H/5g6g indicates a tolerance class of 6H for the nut (female) thread and a 5g tolerance class for the pitch diameter with a 6g tolerance class for the major diameter.

Booze Daily said:

Are you refering to runout?

Click to expand...

Yes.

Booze Daily said:

I'd bore and singlepoint the thread.

Click to expand...

You mean to say you'd turn the thread instead of using a Tap?

Booze Daily said:

A drill and tap could walk.

Click to expand...

Will a thread created by turning be better than that done by a Tap?

Booze Daily said:

I don't think I'd screw it on a bolt or thread gauge and expect any accurate runout readings. There's slop between the mating threads.

Click to expand...

That's what many local expert said but the customer wants it that way and ... he's the king

Booze Daily said:

PS: you might want to change the topic title.

Click to expand...

Done. Thanks for pointing it out.


Neither did I have formal technical education nor English is my first language so please pardon me if my query didn't point in the exact direction.

I know what he means, but I had to actually check a geometric tolerancing handbook to see if there was such a thing as ovality.

Johnny Larue said:

first off a mechanical comparator is an indicator...YES?

Click to expand...

This is a mechanical comparator.

Johnny Larue said:

...make sure you use a center drill at 1st operation to insure tap straight...single point them just a few passes and leave a little stock....now run the tap in and it will follow the perfect threads you have roughed in...then use the gauge to make sure they work good and in tolerances...WALLA

Click to expand...

Currently I am doing following procedure...

1) Clamp the ID 21mm on an expanding mandrel on a CNC Lathe
2) Turn face with 0.2mm stock and finish turn entire OD.
3) Drill the bore 8.3-35mm with a 8.2mm drill bit. The drill is fixed on the turret, not center.
4) Turn the bore to 8.60mm with a small boring tool.
5) Counter bore 11.30mm with another tool that also finish turns the face.
6) Generate the thread using a standard Tap.

Since I am already turning the bore after drilling, do I need to use a small threading tool to rough turn the threads ?

Johnny Larue said:

PS...I assume those threads are 6H/6H....here read this



Thread Tolerancing

A full designation for a metric thread includes information not only on the thread diameter and pitch but also a designation for the thread tolerance class. For example a thread designated as M12 x 1 - 5g6g indicates that the thread has a nominal diameter of 12mm and a pitch of 1mm. The 5g indicates the tolerance class for the pitch diameter and 6g is the tolerance class for the major diameter.

A fit between threaded parts is indicated by the nut thread tolerance designation followed by the bolt thread tolerance designation separated by a slash. For example: M12 x 1 - 6H/5g6g indicates a tolerance class of 6H for the nut (female) thread and a 5g tolerance class for the pitch diameter with a 6g tolerance class for the major diameter.

Click to expand...

Thanks for the explanation. I didn't have formal technical education and Practical Machinist and its members have helped me a lot on my short comings.

mdshunk said:

I know what he means, but I had to actually check a geometric tolerancing handbook to see if there was such a thing as ovality.

Click to expand...

Sorry for the trouble but neither did I have a formal technical education nor English is my first language hence I might have caused the confusion.

Prasham said:

When I check it after fastening it on a screw it shows random ovality of 0.1 to 0.25mm where as the acceptable tolerance is 0.15mm.

Please guide me what to do to get the component in required tolerance.

Click to expand...

Well, since your customer wants it that way, screw it on a bolt and tap the part around to see how true you can get it to run. You're only looking to save 0.1mm.

Besides, how do you know how true the bolt runs?

Booze Daily said:

Well, since your customer wants it that way, screw it on a bolt and tap the part around to see how true you can get it to run. You're only looking to save 0.1mm.

Besides, how do you know how true the bolt runs?

Click to expand...

this is why you MAKE YOUR OWN BOLT...that way customer sees it spinning true on a bolt like he wanted and the threads will be straight and standard....do you need specs for a metric thread? do you have a machinist handbook? and your doing good for no formal training....theres some guys I know had 25 years of schooling and machining cant even square up a block yet....LOL

Prasham -- In many cases, it makes more sense to use the thread as the clamping mechanism (only) and use a straight-bore feature as the "register" diameter. This is the way many older lathe spindles were built, so that the thread for the chuck was not the element creating the position for the chuck, but rather the shoulder on the spindle nose and the recess in the chuck body. This eliminates thread clearance as a contributor to runout.

Your part drawing shows a shallow (unspecified) counterbore at the thread end. If you can control the size of the counterbore closely as awell as the squareness of the small face, you could then thread the tapped part onto a threaded post with a shoulder that fits the counterbore, and finish turn the necessary dimensions with the counterbore as the precision reference. This may take longer to do, but it may also give you what you need for tolerances. OTOH, if you have a CNC lathe doing the work, I would think that with sharp high-quality tooling on a well-set machine, you should be able to get what you want fairly easily. The suggestion about single-point threading may well be the way to go.

Bear in mind that many things can affect runout, particularly where hydraulic clamping is involved.

ON Edit: Also keep in mind that your customer may be KING, but sometimes even the King requires a bit of education about what is possible from a tolerance vs. manufacturing method viewpoint.