[Hood]

Anyone know if its possible to alter the internals of BobCAD so that it will output thread heights correctly for full profile inserts?
The internal calculations are done such that if you were using a sharp point they would be correct but if using a full profile insert then it will cut too deep.
I am thinking it likely wont be possible to alter this and I am thinking I could probably do it via a programme block, but thought I would ask anyway

Hood

[Machineit]

I actually should be the same, unless you have inserts that have radius's on the root point I think. The theoretical points should be the same. The inserts should just clean up the thread OD crests, right?

Mike

[Hood]

The inserts are full profile, in other words they have the full thread form for their pitch (root and crest are cut) thus when BobCAD uses the theoretical height to calculate the finish X it is too deep.
Hood

[Hood]

I am trying to do it via a program block but my VB is crap and I havent got there yet but hopefully I will manage sometime this year

Hood

[Machineit]

The inserts are full profile, in other words they have the full thread form for their pitch (root and crest are cut) thus when BobCAD uses the theoretical height to calculate the finish X it is too deep.
Hood

I understand that, but I'm just saying that it is a matter of knowing where the theoretical tips are and using that for tool dia./offset or whatever.

Hey, you still got 4 months left!

Mike

[Hood]

Well must be getting better, 4 months ahead of schedule I have it working

Hood

[Machineit]

Well great, what did you do?

Mike

[Hood]

Machineit
Well great, what did you do?

Spoke a bit too soon, is what I did
I have it working for the most part but it will output a lot of decimals, so need to find out how to limit them.
Also still have to work out the correct multiplier for my threads but I think they are close enough for now.

Here is the code I used, now dont laugh, I told you my VB was crap

2005. Program Block 5.
StartX = LATHE_Getprofilestartx() *2
Pitch = LATHE_GetThreadLead()
EndX = LATHE_GetThreadX2()*2



If EndX < StartX then
height=StartX-(Pitch*1.32)
Else
height=StartX +(Pitch*1.516)
End If

LATHE_SetReturnString(height)


Hood

[Machineit]

Looks like Greek to me!

Have fun.

Mike

[Hood]

Looks like Greek to me!

Have fun.

Mike

LOL doesnt look much better to me

Hood

[mmoe]

My VB is most certainly worse than yours, but maybe this is another approach. Could you put the math down in the If, Else, Endif section instead? The comparison would still work fine since both are being multiplied and the math would all be done later.


2005. Program Block 5.
StartX = LATHE_GetProfileStartX()
Pitch = LATHE_GetThreadLead()
EndX = LATHE_GetThreadX2()



If EndX < StartX then
height=(StartX*2)-(Pitch*1.32)
Else
height=(StartX*2)+(Pitch*1.516)
End If

LATHE_SetReturnString(height)

I don't really have any way to test it. I also think that the first line was a typo? Probably should be capitols in there (not sure how case sensitive it is).

[Hood]

Dont think that will make any difference but will try and see. Think it has more to do with the string, will have to do a bit of reading and see if I can work it out.
It will be fine for external threads for the most part as they will tend to be round numbers I think but internals will tend to start with decimals.
Its not really an issue as far as Mach is concerned its just a visual thing but would like to get a way round it.
Hood

[Hood]

Just tried and as I suspected its the same

Looks like I have to break out the VB for stupid people book
Hood

[Hood]

Ok got it working

put this just before the last line of code and it limits to 3 decimals and rounds it as well

height = FormatNumber(height , 3)

Hood

[Hood]

Well I think I have it now, I used the very nice thread calculator from Vardex (used it for years and its always spot on) to get different values so I could modify my VB.
Here is what I have come up with, it should work well for me for any 60 degree thread form that I regularly do

2005. Program Block 5.
       StartX = LATHE_Getprofilestartx()
       Pitch = LATHE_GetThreadLead()
	   EndX =  LATHE_GetThreadX2()
	   
	   

    If EndX < StartX then
     height=(StartX*2)-(Pitch*1.226)
	 Else
     height=(StartX*2) +(Pitch*1.17)
    End If
  
    height = FormatNumber(height ,3)
   LATHE_SetReturnString(height)

The actual G76 lines in the PP are

87. Start of thread (G76) cycle
    n,"M49"
	n,"G76","X",program_block_5,thread_z2,thread_lead,thread_first_cut,thread_angle_in,rough_retract_amount,thread_last_cut
	n,"M48"

88. End of thread (G76) cycle
	n,spindle_off	
	n,program_block_2

For metric internal threads the normal way to determine the drill size is to subtract pitch from nominal thread size and that gets you close enough for most things, however as I am turning the thread rather than tapping I want to leave a wee bit extra so the insert will form the crest. I use the formula of pitch *1.1 and subtract that from the nominal thread dia and again it seems very close.
I may end up doing another programme block which will automatically give me the start dia even if my drawing is not quite right but will likely not bother.

One thing I thought about was having some advanced programming options in BobCAD so I can choose the threadform (metric, whitworth etc) and it would automatically adjust the G76 to suit but I thought about it and as I mainly do metric or Unified threads then its not worth the hassle as I can easily tweak the code if I am doing a Whit/BSP or some oddball thread.

Hood

[mmoe]

Nice work Hood!

[Hood]

Well it works great, for external threads anyway
Using BobCAD for the first job today and its worked very well now that I have things dialled in, threading the ends of 25mm dia 316 for pins and first one was spot on so never even really needed the optional stop
The M5/M1 options I have put in the advanced programming is great as it allows me to insert a spindle stop and programme stop after any op without having to enter it manually into the code, was very handy for these 125mm and 100mm dia rollers I made today, again programmed by BobCAD. I had a M5 and M1 after the rough to clear away this mess, I hate nylon

Hood

[TonyW]

Don't know if this will help or not, but it works quite well for me for most applications. When it comes to thread turning, or thread milling, Bobcad seems to just pick numbers, usually too deep. This is Sandviks Threading Calculator for both turning and milling internal and external threads. Shockwave app so it runs itself. Keep in your files for future reference. Tells you pretty much everything for every type of thread and works with other companies inserts and mills as well because it just gives you the cut data, etc. I enter the data from calculator into Bobcad and it makes perfects threads for me every time.

Click here to download: http://www.witznet.net/files/sandvikthreadcalc.zip

[Hood]

Thanks Tony, I have used it in the past but prefer the Vardex one personally, its a bit slower as it searches for tools but it does give you the boring dia for internals, dont think the Sandvik does, then again its a while since I looked at it.
The reason I altered the PP however is so I dont have to look up data and punch in numbers (other than pitch).

Hood