inverse feed problems

[millboy]

I am just going into 4th axis rotary surfacing got the tool path to work ok.My problem is this inverse feed on a haas v2-hrt160 very slow.So messing around using haas genric 4th I post out 20. ipm then 60 ipm on the same file the inverse numbers are bigger on the 60 ipm than the the 20 ipm, downloaded mpmaster post it does the same thing. From what i understand that is a time value so that is backwards. what am I missing ?

 

Help!

 

Thanks

[Peter - Avivi CNC Solutions]

4th Axis brake is off? (M11/M12 I guess...)

[dfedwards]

F(code) = 1(minute) / (time = 3D distance/velocity)

The 3D distance of the move is calculated in model coordinate space at the NC control point, not in machine coordinate space and not necessarily at the tool tip. For example, a 5-inch move at 50 IPM takes 5/50ths of a minute, yielding an inverse time calculation of 1/.1 and an F-code of F10. The same 5-inch move at 700 IPM would be 1(minute) / (time = 5 / 700) or (1/(5/700)) or (1/.0071428) or F1400.168

 

If that's not clear enough, think about it like a record player. The closer you move to the center of rotation, the slower your linear velocity is. Say you are cutting a part by rotating a rotary table, and you would like to feed at 10 linear inches per minute. How can you just give a F10.0? What if the part you were cutting was 30 inches in diameter? What if it was 1 inch in diameter? The controller doesn't know what diameter you're cutting. F10.0 means nothing to your controller. So, to correct for this, we use inverse time feed. Some controllers may vary, but most I've seen are calculated by 'Speed(IPM or MMPM)/Distance)'. For example, you want to move at 10 IPM and your move is 2 inches long. Your feedrate in G93 would be 5. So you can see very small moves give you huge feedrates, expect to see F1500.0 or more. Most controls also need a F on every G01, G02, or G03 line. The F will most likely vary every line.

 

Also, Because inverse time calculations can appear confusing for the uninitiated five-axis programmers, some machine builders have attempted to simplify five-axis programming by offering a form of rotary feed control where the CNC operator manually sets the fourth and fifth axis radius values (this is true on a Haas 4^th axis machine).

 

Hope this answers your question.

[mkd]

http://atyourservice...-feed-mode-g93/

 

 

 

 

This VMC/HMC feature specifies that all F (feedrate) values are to be interpreted as “strokes per minute.” This is equivalent to saying that the F code value, when DIVIDED INTO 60, is the number of seconds that the motion should take to complete. G93 is generally used in 5-axis work, and sometimes in 4-axis work as well. It’s a way of translating the linear (inches/min) feedrate assigned to the program – F30, say – into a value that takes rotary motion into account. When G93 is activated, the F value will tell you how many times per minute the stroke (tool move) can be repeated, based on the linear F value.

Haas has been able to accommodate full 5-axis machining for many years; however, this feature, in conjunction with aftermarket CAM systems and their post-processors, offers even more flexibility and versatility.

 

what you're seeing in your posted code sounds like what Haas says here. larger feed rate= more strokes per minute.

[Mugsy DeDawg]

Hate to mention a competetive product, but GIBBS had a a nice explanation of inverse time feedrate on their site years ago. Basically, if you are moving 1 inch per minute feed, and you make a 1 inch move, your feedrate is 1.0, if you move, your feedrate is 2.0, and so forth. The reason it is good to use in 4th or 5th axis is that it gets rid of the issue of which feedrate you are using, degrees per minute, or inches per minute. It does create a lot of code, as you basically have a feedrate for each move.we used it successfully when making a dovetail slot on the outside of a rotary valve witha a X/A move at a fixed Z and Y position, wrapping an elipse around the body. It made a smoother cut and got rid of noticable changes in sound of the cut as it fed around the part, which was also shown by the finish. The limit like with degrees per minute, is how large a feed number you could put in. The applications people with the control, the machine, and the 4th axis head were all unable to give a definitive answer, and gave the answer, "I would keep increasing the feedrate until it alwarms." Hope this helps.