Edgecam Translate Output Subroutines

[jtreanor]

Hi Everyone,

The trick to getting the subroutine to output correctly is to manually
add a couple rapid moves to position the tool just before the instruction
to be translated.

We all appreciate not having to manually enter rapid approach moves
for every instruction, the drawback in this situation is that they get
copied in a translate.

a single mill cycle will automatically output a rapid approach move
that does not appear in the instruction list.
when you "Translate" the instruction the automatic approach move
will translate also.
In the example the second rapid Z approach move is to the same
"Clearance" level set in the translated profile cycle.

I certainly agree that it should be documented somewhere,
and the help files aren't totally useless -
only for the help items I'm looking for.

Jim Treanor

[GazMann]

This got me the first few times I tried the translate command. The same thing happens in matrix mode. If your previous cycle before the cycle that you are trying to transform was a toolchange, the transform will lift to the Z height as specified in the toolchange position in your post. This sometimes results in an overtravel in Z and at best excessive Z moves between translations

A little trick I was shown was after you have created the toolpath you wish to translate, select rapid move and when prompted to digitise end point for move, hold down the ctrl key ans select the bottom of the rapid approach toolpath above the job. This will select the coordinates of the rapid move to clearance. Then drag this to below the toolchange and above the first SYSLABEL. This gives a set of coordinates for the translate command to start each translation from

[jtreanor]

when ANY Edgecam instruction asks to digitize a point or coordinate,
a digitize on screen will return all 3 XYZ coordinates,

pressing the keyboard keys X, Y, Z or A(bsolute) or I(ncremental)
will open an input window where you can type in the desired
coordinates if there is no point or geometry to click on.

in this case getting a rapid move to ONLY output the Z portion
requires typing in Z.25

[GazMann]

True Jim but until you have created a toolpath that you wish to transform you do not know where you need to rapid too. By creating the toolpath first you are able to determine where the rapid move is from toolchange to clearance. This is shown by a dotted line leading onto the job. When you are asked to digitise the points you are able to hold the ctrl key and select this initial rapid move in the display. This will copy the end coordinates of that move into the rapid move that you are creating. I don't know if I am making sense in what i am trying to discribe.

Something else you can use is from the move menu select initial plane, as long as your post is set correctly.

[jtreanor]

Hi GazMann,
I have 2012R1 and cannot select / digitize a toolpath, rapid
or other move as an input for a new Rapid move end point.
(probably a preference / selection setting somewhere)

The point anyway is that it would return all 3 XYZ coordinates
as the end point for the new rapid move.

If you want a Rapid move that outputs ONLY a single axis move
- G00 Z.25 - you cannot digitize on the screen
you can manually enter the single value by typing Z.25

there are probably other ways to get around it also,
I just find the manual entry method the simplest.