Using G01 alongside G00 (slow feed rate woes)

[inthezone]

So I have a Fanuc OM controller, fairly standard you might say. FeatureCAM offers a default post for this exact controller.

I am running into a problem with FCAM calling up a G01 for Rapid travel as well as a G00. I immediately get an error with my program because it doesn't bother to include a feedrate for the G01 (which requires feedrate). That is an easy fix, because using MDI mode, I can specify a feedrate manually and the program works fine.

But it's still a problem because every time there is a tool change it calls for a return to reference position Z0. That works fine in rapid travel mode, but when it returns to the part, it calls up a G01 in the same block as G00, and it uses the last feed rate commanded.

That means if I was doing a pocket at a feed rate of 2 ipm and then I go in for a tool change, the bit raises above the part at rapid travel rate (which is no problem), but then when the bit comes back down to the part (since it calls for a G01 alongside the G00) it comes down at the previously specified feedrate (as if it were doing a huge plunge) OF 2 ipm which is INCREDIBLY SLOW.

G01 is used for removing material according to the books that I have read. Why on earth is FCAM calling up G01 alongside G00?

%
N25G00G17G40G49G80
N30G30G91Z0
N35T2M6
N40G00G1G90X15.8535Y7.3214S1604M03 <--Why is it calling for a G01?
N45G43H2Z-8.26
N50Z-8.8751
N55G01Z-8.9651F4.8 <--This G01 makes sense

[dcrace]

Notice its G1 and not G01...From the sample code you posted, looks to be outputting the work offset as "1" instead of G54/G55 etc..
look at your setup properties and see if the "fixture ID" is set to 1, if so , try changing it to 54 and re-post code.
Also check the post file, under the CNC-info list, check fixture ID, it should list all of the available work coords. Ex:
54
55
etc...
If you still have trouble I can forward you the post I have setup for the O-M.

[Al_The_Man]

I think you have a problem with your post, as there should not be a G01 and G00 on the same line.
BTW G1 & G01 is the same command.
Al.

[hilldf]

It certainly sound like a post issue. What FeatureCAM version are you using? I may have an OM post I can give you. I program OM controls daily. The post I have works well, but more importantly it may give you something to compare to, so you get an idea of what to alter to get things the way you want. I have never had a "box" post work well in any CAM system I have used. Also, you may want to contact FeatureCAM (They will tailor a post free of charge) or post on the FeatureCAM forum.

Dan

[inthezone]

I changed the setup number to 54 and that changed the number in the code. But why would I need to call up a G54? I actually just manually edited the code and removed all of the G1's and it runs fine.

i will run it tomorrow with the G54's in place..