Rotating NCI

[Hugh.Venables]

Had a job the other day that had 18 pockets arranged radially. Tool pathed one and used rotate NCI. It looked fine in Verify but the posted code started every pocket from the same co-ordinates but with the first relative to G54, the second to G55, the third to G56, etc. I am pretty sure we only have eight G5*s so 18 was going to be a bit of a problem and they were all needing to be calculated and entered so I gave up and chained every pocket. I suspect this is a post processor problem. Any ideas?

Hugh Venables, Monash University.

[Lucky]

Make sure you select "Coordinate" instead of "Tool Plane" as the transformation type. The default is "Tool Plane". Does anyone know how to change this default?

[Hugh.Venables]

Thanks Lucky. That seems to work OK. What does by "tool plane" mean? When would you use it instead?

Hugh Venables.

[Lucky]

Use "Tool Plane" if you wish to transform your pattern using multiple work offsets (G54, G55, etc.). I prefer "Coordinate" transform. It has fewer limitations and simplifies things at the machine (only one "zero" to set).

Does anyone know if it is possible to make "Coordinate" the default setting in toolpath transformation?

I have made a number of bad toolpaths by not being careful to check this.

[Zero]

As far as I can tell, you can't change the defaults in the toolpaths transform menu.I know that you can change all of the regular toolpath defaults by going to screen->configure->NCSettings->Operation defaults,then choose defaults .df8 and a list ofn all the operations comes up.By opening the parameters of each you can change the defaults like filter settings, stepover or down, etc.It takes a little bit of time but I changed most of my operation defaults in here to settings that I use most of the time and it saves me a lot of clicking and typing nowadays.But like I said it seems that you can't change the transform defaults.If you right click the screen the popup menu comes up but transform along with a couple of other things is greyed out and you can't choose them.If anyone else knows of another way to get at the transform toolpath default settings I too would greatly appreciate the knowledge.

[Luther_Heggs]

Version 9 can.

[Elad]

I have the same problem (G54,G55 etc.) when i work with the 4 axis.

Every time i rotate the cplane and the tplane,i get a new wcs.

I use mpfan post,i heard that in mpmaster the problem was solved in the misc value "lock on first wcs"

I didn't try it.

I don't have the time to edit the mpmaster.it took me a lot of time to edit the mpfan for my needs.

I think i'll just wait for the new mpmaster for v9,(i heard that Dave is working on a new one )

[ 12-22-2001: Message edited by: elad ]

[gstephens]

Elad, you need to set the work offset to something other than -1. This is the default setting (which you can't currently change) and ends up outputting incremented workofs numbers (0,1,2,etc) to the .nci file for posting. If you go back and go to T/C planes in your tool parameters and change the work offset in all of your toolpaths to 0, you'll end up with 1 work offset in the output.

[McRae]

Elad - I heard of this post

Currently it is "MPMASTERBETA"

(Say it outloud quickly...)

MfgEng

[Allan Brown]

Beta 9 testers may download Mpmaster9.

 

[ 05-02-2002, 09:49 AM: Message edited by: Dave Thomson ]