[TimBrex]

OK well to start I'm new on here, but anyway when im posting out my program to do an arc in the XZ or YZ axis it won't post out the G18 or G19 command .I have tried different posts , tried the arc filter but it still keeps giving me the point to point on the arc resulting in a "faceted" looking part, Which isn't good . Since we are using ver5.2 and not on maintenence anymore they (Surfcam) won't even let me get past the receptionist, unless we get back on maintenence. what do i need to edit in the post to have it post out the G18/G19 commands?

[mariojl]

The easiest way to do is to have 3 ddifferent post, one for each plane, G17, G18, and G18
Just get to your Postform.m, copy the entire post you're using for your machine and paste it twice bellow the former, name it diferently, for instance "name FANUC G17" / * G18 / and * G19.
Then you must edit the last 2 posts; at the 1stToolChange find the line that reads something like "G<40> G<90> G<17> G<Work> X<H> Y<V> " and replace the G<17> by G<18>, making sure change every G<17> statement; and then proceed with the G19 post.
When you run a job with arcs in XZ or YZ plane, post it with the related post.
This procedure is also needed when the job is done in a machine that can orientate the spindle at diferent planes. I mentioned "Fanuc", but it's the same for any machine you may have.
Hope have been clear enough, have doubts?, just ask.
Mario

[TimBrex]

Mario that might work if i was doing just the one direction , but the part i was working on had both G18 and G19 moves ,which i ended up programming by hand . for future jobs like this i would like to have a post which would output the correct commands ,thanks for the input though.

[mariojl]

Hi,
I believe you’re just trying to get the impossible. Let me try to explain:
When in SURFCAM, and want to NC 2 axis contour a radius in ZX axis, you MUST change the settings to Cview = <2> ( or Cview = <3>) and Coord = View. Is it Ok?
To work in YZ axis it’ll be Cview = <5> or <6>. All the same happens if you want to use drilling / tapping cycles. As a matter of facts, you can work in any plane (angle / CView) you might have created.
In any of this cases, SURFCAM lets you machine in any side of a part without moving it, just change your settings. But regardless the settings your *.inc output WILL ALWAYS BE the spindle being the Z axis.
Now take this to the Mpost, and it doesn’t have any function to recognize Cview plane. And here comes why you need 3 different posts (or more), one for each working plane. In it, the trick is to swap the axis, according to the worked plane.
They’re very useful in machines with swivel heads, or equipped with right angle attachments.
Now if what you want is to contour an arc in XZ plane using a ball end mill in a VMC, ( as cutting a grove) then you have to - "Create / Spline / Elements "- using that Arc, and cut it with "Contour 3D". This way post it in regular manner, because your Inc is output in very small segments of G01; no need to post G18/19.
The other option is having a 5 axis machine, but then in SURFCAM, under NC 5 axis, there is no G2/G3 function.
Should you have any doubt, just ask.
Mario.

[Anders6612]

If you are using Mpost, make sure that you have
this in your post:

ArcPlane g 17 18 19
CtrCode I J K

And in toolchange, in some systems G17 must be present for
the Lcomp to be in Z direction, before G43 H code so
add G<ArcPlane> in toolchange and 1st toolchange.

Example:

ToolChange
G40 G21 G17
M5
M6 T<Tool>
G94 G90 G54 S<Speed> M<Direct>
G<0> X<H> Y<V>
G<43> Z<D> H<Tool>
G<ArcPlane>
end

This works great when i use arcfilter for posting, you also can add
a ArcCode sequence in the processor.