Opposite Parts

[Master Whidbey]

Ok, I do a lot of parts that have a drawing for one side and customer wants the opposite side. Mirror doesn’t work for all. Is there anyway MC will let me draw it one way and machine the opposite?

 

Thanks for all the help

[Zero]

You can tranlate/mirror/rotate your toolpaths. HUGE time saver on complex toolpaths. Right click in the operation manager and select toolpath>transform. I use it all the time...although its a little buggy while using the WCS..v9.1 where are you???

 

[ 02-19-2003, 12:41 PM: Message edited by: Zero ]

[Scott Bond]

Master--nice name

What Zero said and maybe, heres a couple of

other standard approaches.

quote:

---

Mirror doesn’t work for all.

---

Do you mean in the control ?

 

If I have already programed the part, I go to the (fill in machine name here) and turn on the x mir.

 

If it's on a machine that is combersome to mirror,,,I go back to my MC9 file and----

mirror everything,, then operation/geometry/reverse direction,,,regen then post.

 

If it is a new part,,, I draw the part to the print given. Then mirror that part,, then program it.

 

IMHO one of these should work.

[Guest CNC Apps Guy 1]

I mirror things often.

 

If I have to make say a right AND a left, I'll program the shown part first, prove it out. Save, yadda, yadda, yadda. Then I'll save again as a different part number (ex. 12345678-2NC) then I'll go to top view in the WCS and mirror about a line and move everything. Now, I go into the WCS, re establish my Origins, then I go into my Operations Mannager and reverse the chains, etc. I've found inconsistent results with the Transofrm Mirror. It works Bang Zoom sometimes and is just a plain headache other times. A lot of the parts I do are "swoopy", not much flat anything any where so that may have something to do with it, or maybe not. I've not had time to investigate so that I can tell [email protected] what the issues (if any because it's entirely possible I'm an idiot and am not using it correctly) are with it. The way above works 100% EVERY SINGLE TIME, but it is tedious because you have to go through every toolpath and reverse things, make sure your start points are where they should be etc.... So I've been doing it this way.

 

HTH

[Fig sign]

I am with James !

 

I had`t chance to do TRANSFORM->MIRROR IN VER9 ,

but in 8.1.I did a lot and what I found was:

1.If you have jobs of kind contour or pocket and choose an option to preserve the direction of milling ,then you have a big chance that in the transformed nci file arc can be output uncorrect ,especially lead in and out arcs.

If you don`t choose this option the chance is far lower but still exists.

2.If you have surfaces of kind revolved than in

transformed file you have a chance that you mill will cut THE REAR SIDE OF A SURFACE !

So I don`t take a chance.

I simply save the file by other name and thansform

the model and regenerate it .

That`s really fast and safe process.

[Marty A]

hello master i agree with james, iv'e been only programing a short while but i do exactly the same way james does. seems to work for me every time.i'm using 8.1.1 motty

[Zero]

quote:

---

I've found inconsistent results with the Transofrm Mirror. It works Bang Zoom sometimes and is just a plain headache other times

---

Yeah I know what you mean James. It's always worth a shot to try it though...for me anyway. Especialy if your toolpaths take 30 min or longer to generate. The toolpath mirror takes all of 5 seconds to complete. I always verify the posted code afterwards as well to check for those arcs that for some reason or other get reversed.