Mirroring NC path best technique

[DaleHvizdo]

I am wondering what is the best technique for mirroring a toolpath with same cutting conditions. We machine alot of mirror parts that are too large to machine parent at the same time. We need to keep all cutting conditions the same. upcuts, climb cuts and also with surface milling. If we mirror the steps u cannot suppress parents. Is there a way around this?

Thanks

Dale

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[ptc-21369]

Most engineers have never looked at a machine tool manual, it is just not something we have ever had to do. Our post processers are written for us, we never have to think about issues like this too often. But machine tool controls have the ability to mirror a whole program with a simple M- function about the x or y axis or both at the same time. These functions may have some rules that will have to be followed like being at the machine x and y Zero locations. Some machines have the same ability to rotate and scale as well. You can even go as far as nesting your working program as a sub program relocating and re-zeroing your machine a multitude of times. This is all very old school and seldom even considered any more. Get your books out and read a little about it.
Don’t get me wrong on this, I really appreciate the that Pro-Man has all of the abilities it does to pattern and simplify our work. I would rather let the computer do the thinking. It sound as if though you have some machine limitations that are impeding this. You may have to be creative!
Best wishes,
Ronald L. Swift
Engineering Supervisor
Zirc Company
3918 Highway 55 SE.
Buffalo, MN. 55313
763-682-6636
763-682-6604 Fax
rons@zirc.com

[SteveLucas]

Ronald,

Most of the features you speak of on machine tool controls are options that
cost more money(usually thousands of dollars). That sometimes is hard to
justify to bean counters when purchasing a machine when you have software
that will do the same thing.

[rdowns]

Dale,

One thing to consider when mirroring a program is that the "climb cuts"
become "conventional cuts" and vise-versa. Often you will not get the
desired results.


Roger


_____

[ptc-1932745]

It may have been said already, but mirroring the program by multiplying
an axis by -1 will cause climb cuts to become conventional cuts unless
reverse spiral tooling is also used.



Also, since the tool change position does not change, make sure the tool
clears the part / fixturing / tool probe when mirroring.





Christopher F. Gosnell



FPD Company

124 Hidden Valley Road

McMurray, PA 15317

[kevin_marett]

I think it was back in WF3 that ProMFG gave you the option to output a
mirrored sequence and decide if you wanted to keep the existing cutting
condition or allow it to be mirrored.

Simply select "Machining" "Utilities" "Mirror NC Seq".

Regards
Kevin

[ptc-596318]

I did forget about this option. Yes it is still available in WF4.

Also select the mirror plane!!