Underfeeding Tap Cycle

[NYMike]

This subject has probably been covered here before but anyway here it goes.I would like to override the feedrate on the tapping cycle for mastercam. I would like to underfeed by 2-10 percent and let the axial float of the tapping head make up for the difference in depth. This allows the tap to cut cleanly relative to its pitch. Everytime I change the feed, Mastercam adjusts the spindle speed. I have thought of changing the pitch of the tool by the percentage I want to underfeed by, but I thought there might be a better way.

Thanks, Mike

 

[ 02-19-2002, 12:31 PM: Message edited by: NYMike ]

[Mgrenier]

Hello NYMike,

 

I would personnaly go touch my post processor for that matter. You can adjust your feed in the ptap post block by multiplying the feed given in MC by a fixed number all the time. And if you want to control the multiplying factor in MC, I would use the Real values.

 

Hope this helps

[NYMike]

Martin,

Thanks for the advice. I am not familar with changing the post yet. If anyone out there knows of a book outlining post modification please post a link.

Mike

[Chips Ahoy]

The post cd is o.k. It should help. It was only around 10-20$ Pricing will fluctuate with location. Thought I would put that in here because some people don't seem to like us posting prices in here.

[Smit]

You could create a tool with the speeds and feeds you like and save them to a tool library to pull up for future use. I believe that is easier to do for somebody who is unfamiliar with working with posts. Right clicking on the tool in the operation will allow you to adjust and retain the feeds and speeds also. But when changing the feed on the parameter page Mastercam will automatically change the speed too.

 

[ 02-20-2002, 07:22 AM: Message edited by: Larry Smith ]

[P_Scott]

NYMike,

 

Larry's idea is a good work around if used in conjunction with the Job Setup switch stating "From Tool" under Feed Calculation. That way whatever feed is saved with the tool parameters, Mastercam will use that value instead of calculating from the material. You would have to change other operations for the other tools, or make sure other tools had correct feed rates in their parameters as well. "From Tool" feed calculation will do it for all the tools in all operations. HTH

[NYMike]

What I did for this situation was create a tool for a 5% reduction in feedrate. The actual tool was a 1/4"-20 Tap. I created a tool with 21.05 threads per inch (1/4"-21.05 TPI). Mastercam calculated speeds and feeds for material specified and this did not effect the speeds and feeds for the other tools in my operation.This gave me the 95% feedrate I wanted when using my 1/4"-20 tap. I saved this tool as a 5% underfeed tool for 1/4"-20 and if I need to do this again I can call up the saved tool. Thanks to all for your advice.

 

Mike

[Glenn Bouman]

I think the easiest way is to change the post.

Under ptap add this line

 

code:

---

     feed = feed *.95  

---

 

[ 02-20-2002, 06:55 PM: Message edited by: Glenn Bouman, In-House ]

[JS]

Thanks Glenn

 

Nice tip, I like that!

 

Joe