Programming a metric tap when in inches mode

[krosen]

I have a job that I need to program a metric tap (which is unusual at our shop).  I selected a metric tap (when in inches mode) and thank the lord I ran the tap a couple inches above the part on the first hole because it wouldn't have been pretty.  I then read online that in order to program a metric tap in inch mode you have to use an inch tap and convert the tool geometry to metric.  is this correct? or is it possible to select and use a metric tap when in inch mode?

[Guest]

Search the forum, I shared up a metric tap library all converted to inch

[krosen]

Thank you will do

[jlw™]

For the record, I use JParis' tool db but when I need to know the conversion or what not I hit this link:

 

http://www.newmantools.com/tech/pitchconversions.htm

[Tim Johnson]

m3-.5 tap -- 1/(.5/25.4) = 50.8 threads per inch

[gcode]

I just go to the thread per inch field of the tool definition and enter

 

1/ (metric pitch value mm) and let Mastercam do the work

 

so for a 1mm pitch thread

 

1/(1mm) = 25.4 threads per inch

 

a 1.5 mm thread would yield

 

1/(1.5mm)  = 16.933333 threads per inch

[Colin Gilchrist]

When you output the Feed value for a Tap, it's very important to check the format being output. Many times the control will accept 5 or 6 decimal places for a Tapping Feed Rate, but the output in the post might be set to 3 or 4 decimal place output. This can mean a slight error in the synchronization between the spindle rotation and the Z feed, which can cause a loss of precision in the tapped hole, and I've even seen where a 3 place decimal caused enough of a lead error to break a tap.

[civiceg]

Which is why I will adjust the rpm of the tap, to get a non rounding decimal. Regardless if its metric or not, I will get a whole number output for the feed or minimal decimal places.  

[crazy^millman]

Which is why I will adjust the rpm of the tap, to get a non rounding decimal. Regardless if its metric or not, I will get a whole number output for the feed or one decimal place. 

 

That could be in your post. Have you tired a generic post and see if the output is different?

[BrianP.]

I just select the tap I want from the metric data base. Change feed rate to whatever I want and Mastercam will do the math. Select an M3 x .5 tap while in inch. Change feed field to 10IPM and Mastercam automatically changes RPM's to 508.

[mikenaturalice]

Which is why I will adjust the rpm of the tap, to get a non rounding decimal. Regardless if its metric or not, I will get a whole number output for the feed or minimal decimal places.  

This is what I do too. Convert the metric to inches, then play with rpm to get a whole number for feed, or maybe just one decimal place.

[Mjölnir]

I just go to the thread per inch field of the tool definition and enter

 

1/ (metric pitch vale mm) and let Mastercam do the work

 

so for a 1mm pitch thread

 

1/(1mm) = 25.4 threads per inch

 

a 1.5 mm thread would yield

 

1/(1.5mm)  = 16.933333 threads per inch

 

exactly what i do for building molds / tooling with metric components.

[Thad]

This is what I do too. Convert the metric to inches, then play with rpm to get a whole number for feed, or maybe just one decimal place.

 

Why bother?

[jlw™]

The theory is pitch error. However, no deeper than *most* taps go I wouldn't worry about the 2nd or 3rd decimal places. I have seen the pitch finally stack up on holes that were threadmilled really deep but I also thought they were threaded way to deep. JM2C

[civiceg]

I look at it this way, if you are going to make a tap library, might as well make it so rounding doesn't ever come into play. Programming in in/min btw. 

[Thad]

I guess I've just been lucky. I've tapped 1000s of holes over the years and never seemed to have broken one because of pitch error. Maybe I was getting premature tap wear because of it and then when it finally broke, I chalked it up to a dull tap.

[JAMMAN]

I just go 25.4/metric pitch and enter it for taps pitch. Never thought about using a metric tap library. Maybe I'm under thinking it.

[jlw™]

Whatever works. Always more than one way to skin the cat. Some people start at the head, others at the hole.

[huskermcdoogle]

feed per rev just simplifies things so much.......

[So not a Guru]

I just go to the thread per inch field of the tool definition and enter

 

1/ (metric pitch vale mm) and let Mastercam do the work

 

so for a 1mm pitch thread

 

1/(1mm) = 25.4 threads per inch

 

a 1.5 mm thread would yield

 

1/(1.5mm)  = 16.933333 threads per inch

Awesome! I didn't realize till this post that MC interprets the "mm" automatically in entry fields. Thanks.