[E300]

Good day all! I'm gonna do my first thread on my LB-15 OSP-5000L. I understand this threading canned cyle "G71" except where the "H" value come's from, meaning....I know its the height of the thread say major dia' minus the minor diameter divided by two for the "H" is the radial height.
I'm using a 60 deg "POINTED" "OD" threading tool...my question is... Okuma machine threading cycle looking for the "H" value as sharp point (Major Diameter) to sharp point (Minor Diameter) dimension as indicated in the attached picture? Or major diameter and minor diameter as indicated in the Machinery's Hand Book?
Thanks so very much for any help

[E300]

I'd doing a M22 X 1.5 - 6g

If someone can give me the "H" value for this thread and how you got it would be greatly appreciated

[deadlykitten]

i master threads please share :

... insert nose radius
... insert type : full or partial
... thread length, or better, full part drawing, and i will give you a code an explanation as best as i can tomorrow, of course, since my work day finished a few hours ago

[E300]

Hello "deadlykitten"

1: Sharp point threading insert.
2: Full insert
3: 30mm long thread (M22 X 1.5 - 6g)

[deadlykitten]

full insert should not be sharp; please check again if you wish, use attached image as a reference, for example, an insert for 1.5pitch has 0.19 radius

also, please provide "s"

you may edit start-end positions any time if you are ok with this, than skip next part :

about the 30mm length :
... should the tool continue moving ? thus, is there some clearance after those 30 mm, and tool will move until Z-35..-40 for example ?
...... or
... "-30" is fix ?
...... or
... "-30-s" is fix ?

is the thread starting from part frontal ? a drawing may avoid all this question

[deadlykitten]

I'm using a 60 deg "POINTED" "OD" threading tool...my question is... Okuma machine threading cycle looking for the "H" value as sharp point (Major Diameter) to sharp point (Minor Diameter) dimension as indicated in the attached picture? Or major diameter and minor diameter as indicated in the Machinery's Hand Book?

inside G71, H/2 is the depth of the cut, or how much the tool is programed to enter inside the material

this H value has no direct (absolute) connection with the picture that you post; is only same notation ( same letter ), reffering ( relative ) to thread shape

[deadlykitten]

the H that you should program, since you have a full insert :
... his value depends on some things and "c", as shown in attached image
... his positions depends on other things

is not necessary to know all this "things"; some X offset corections should deliver your thread

the image that you post is a zig-zag designed some decades ago by an ancient greek .... if you change it a bit, it may deliver threads / gears / broaching tools

[deadlykitten]

designed some decades ago by an ancient greek ...

this guy decided to build a water pump so all artists to continue painting / carving, without the need to carry water buckets / bags

result was that all artistic steped into next level, sculptures showing a more relaxed position, more human kind

the artists remained in history, while this "inventor" vanished, but he was "viral" while he was alive, when all artists became famous after ....

[OkumaWiz]

Use the numbers from the machinist handbook. The H only determines the start point for threading in reference to the bottom X dimension of an OD thread in your G71 line. This will determine the number of passes depending on your D value. The larger the H the more passes it will take and the farther away from target in X that it will start it's first pass. It does not have to be accurate, but too small and you will take a "heavy" first pass.

Best regards,

[deadlykitten]

I'd doing a M22 X 1.5 - 6g If someone can give me the "H" value for this thread

recomandation for full insert :
... d2 : od after threading : 21.92 [ -0.091 .. +0.049 ] [ mm ]
... d1 : od before threading : d2+0.16 [ mm ]
... H = ap 1.03 [ mm ] : 26 24 21 16 11 5 [ mm/100 ]

final dimensions is d2, while d1 is an intermediate

however, for stable results, tolerance for d1 should be as "tight and comfortable" as your cnc can deliver

how you got it would be greatly appreciated

please, upload a drawing with your insert

[broby]

I do believe Kitty that the Wiz's answer is spot on and all that is needed. Why do you need a picture of the insert?
Put simply, the H value is used to control the depth of the FIRST pass, just as Mr Wiz stated.
Once again it looks like you are over engineering your answer.

[Superman]

Once again it looks like you are over engineering your answer.

Nah....he's just creating a problem to suit his answer....or...... is that everyone else's problem, from his answer ( something like that...er... now I'm confused )

[deadlykitten]

E300 has exceeded their stored private messages quota and cannot accept further messages until they clear some space.

[deadlykitten]

hy Broby, long time no see ... where have u been ?

Why do you need a picture of the insert?

different insert geometries come with different toolpaths

Put simply, the H value is used to control the depth of the FIRST pass, just as Mr Wiz stated.

ask him again D is used for 1st pass

[deadlykitten]

different insert geometries come with different toolpaths

generally, this is solved by messing with X_offset

the bigger the difference between "insert shape" and "desired/theoretical thread" , the bigger the "correction"

thus, "thread inserts" require bigger corrections than "turning inserts"

precise H value is relative to insert shape, thus if someone would ask me how i would determine this value, i would need the insert shape

[E300]

Hello all!! Sorry for not getting back to you's... Briefly, I was let go at my day Job of 28yrs but good news is the LB is my machine Here are the pic's DK was asking for....Thanking you all so much for your supportAttachment 337222Attachment 337220

[deadlykitten]

hy e300, i am really sorry for the job lost ... also, did u receive an LB when u were fired, as a consolation ? or how did you get that machine ? if you were able to buy one each time you received your salary/retribution, than pls try to go back to that job

i am just joking

now, about your thread :
... i saw that drawing : [ M22x1.5 x 26length ] [ o18.5 x 14 ] > this is enough 4 me
... do you intend to craft your part with the M22x1.5 :
...... towards the spindle ? so part will be like in the drawing ?
...... towards the tailstock ? so part will be like drawing "flipped" ?
... that is a partial insert do you have a full insert ?

thus :
... if you have a full insert, please share data/geometry
... if you don't have, and you wish to use this one, than :
...... please, how do you intend to verify this thread ?
...... wait until i will get to work, so to give you :
......... dimensions before threading
............................ after ...............

now, some theory : advantages of full insert compared to partial :
...... final thread is easier to control, because full insert cuts also the external diameter, while a partial cuts only on flancs; thus, after a full insert, you may measure only the external diameter, while on a partial insert, the external diameter is cut before by a turning knife, thus measuring it will not give you relevant data about the thread
...... better surface near the external diameter, because the full insert will cut it; a partial one may increase the external diameter because of plastic deformation during cutting; in other words : a partial insert will get wear and will start aplying plastical deformation near the external diameter, so you should change the insert; a full insert may continue without problems if it gets the same ammount of wear ; this depends ( on material hardness for example ), but reality is not far from what i said
...... lower H / yes, a full insert cuts less material, on radius why ? because partial insert have a smaller nose radius, thus they must go deeper into the material to deliver same thread section

how to minimize H on partial inserts : minimize external diameter before threading of course, this thing is not always required, but is good to know just in case ...

[deadlykitten]

please take a look at attached image :
... a partial insert cuts the blue shape ( flancs ) after the external diameter, yellow, was turned before
... a full insert cuts bought blue + yellow

the black contours are for the GO, and noGO calibers

thus, for a full insert, you may decide how much to raise the flancs by measuring the external diameter

for a partial insert you can not do that, thus you must measure the flancs with another method

most common, you verify a thread by the GO and noGo calibers; this calibers have a tolerance T

on a full insert you can know precise where is the thread located inside the T tolerance

on a partial you can not know the location of the thread inside the T tolerance, unless you measure the flancs

generally, Go and noGO calibers are more than enough, but sometimes the client may request to reduce the T, thus to achieve a smaller play between the screw and the nut

in this case, a full insert will help hitting the smaller T faster, while a partial insert may require wires to measure the profile

so try to make a stock of full inserts, and but partial only when you can not deliver a thread by using a full insert


of course, i will help you with dimensions for the partial insert that you have, but only on Monday

also, you may cut the thread without this dimensions, only by using X_offset corections, until GO and noGO calibers are ok

... is easy to cut that thread only by using X offset corections
... is easy to program the machine with the dimensions that i will give you
... it takes time to understand how those dimensions are calculated

thus, you will lose some time to get this knowledge, during which you may craft a lot of parts your choice

[E300]

Good day DK, just came in the house from the shop to read your message

[E300]

Thanks DK, I have to cut these threads today/tomorrow and deliver Monday. So I will try with what I've learned now

1: Only inserts I have are what I showed you.
2: Gonna turn thread from tail stock to chuck, flip part and do the same to other end.
3: I have customers nuts to fit my OD threads required but also have formulas for three wire method.

PS: Love Okuma so I was lucky to find this LB-15 in nice shape and had to buy it