Correct way to copy tool path?

[neurosis]

Im not even sure if this is the right question to ask. I have some parts to make that are very similar. They are as shown and opposites but with some other differences as well. What I am trying to do is copy tool path that i used to create the original part and just re-define some z-depths and change some hole locations to fit the different dash numbers. Ive tried to both create a new machine group for each dash number and copy the tool path to the different group and ive also just copied it to another toolpath group although I liked it better separated in to machine groups (look more organized although not necessary). Every time i get the path copied and re-defined (mostly z depths changed) when I close the part file and open it later the path is all dirty with missing geometry. Anyway, enough of the book. What is the proper procedure to copy path and insert in to other machine groups and/or toolpath groups?

[Dave Ball]

What version are you running? Are your parts solids? There is a known bug in X when you copy operations. The copies tend to revert back to some of the original geometry. This drove me nuts for awhile.

[neurosis]

Im using X2 sp1 I believe. We are in the process of catching up our maintenance right now so soon it will be x2 mr2 hopefully.

[gcode]

Put the Red Arrow of Doom where you want the copied toolpaths to land,

Then select the source files and right click/copy.

Place the cursor on the RAofD a right click/paste.

Works great in X2_MR2... Worked great in X2 as

well

[Colin Gilchrist]

Neurosis,

 

Typically the most reliable method is as follows:

 

Create a separate copy of your "as shown" file. Rename it to the opposite hand part number. Now turn on just your solid/surface model and use bounding box to create a center point. Then create a vertical or horizontal line (depending on how you want to mirror the part) using that center point.

 

Then turn on all your solid/toolpath geometry (turn off anything that isn't moving like your stock and fixture geometry). Now select the mirror line and press the "invert selection" button on the general selection toolbar. Now choose Xform - Mirror and choose the option to mirror about the line.

 

This will mirror all of the necessary geometry, but will also tend to flip the side/direction of all your 2D chains. Surface machining operations (3D) will regen just fine.

 

Now for every contour operation (pocket doesn't matter), expand the operation in the ops manager, click on geometry, and do this on EACH chain:

 

Right-click on the chain and select "Reverse Chain"

 

Then Right-click again on the same chain and select "change side".

 

This will allow you to keep the desired climb milling direction.

 

As you continue to update your operations you might need to switch lead in/out values and make other parameter changes in addition to adjusting the geometry.

 

Why do I use this method? Doesn't Mastercam have Transform toolpaths that do this? The answer is "yes", but I've found them to be un-reliable at best. The other thing that ends up happening usually, is that your setup locations can get screwed up. Not to mention trying to mirror toolplanes for a 5 axis part (that gets ugly real fast). The main reason I use this method is that it is 100% reliable. Once you mirror the geometry and make your changes, nothing is going to revert or do something ugly on you. I also tend to generate surfaces for my machining operations because they mirror much better than a solid when used in a toolpath.

 

HTH,