Surface Rough Flowline issue

[killall-9]

Hi Guys,

I cant seem to get around this op selecting my whole part, rather than a surface (which is the curved chamfer surface)

 

Ive selected the imported IPT as the solid material. Am i missing something ?

[jlw™]

Are you creating individual surfaces or picking on the solid?  If picking on the solid, make sure you only pick one face by turning off the "whole solid" selection.

[killall-9]

Hi Jlw, when attempting to only select the curved chamfer surface, it auto selects the whole part..

[jlw™]

Did you uncheck this box:

[jlw™]

I'm a little old school too, I'd just create a surface from solid and then pick it.

[killall-9]

Jlw,

 

Thanks man !

 

last question, how can i start off the part, im new to this operation and as you can see i extended my lines to do this.

[jlw™]

Click the direction check box, then the direction button, in there, for #1, this is an angle from the X axis, I usually set it to 0 for a "flat" lead in.  #2 is the length, i usually do half my tool plus the clearance I want, #3 is about what direction.  I pretty much always use cut direction but a few people I have talked to prefer about x axis.  Play with it a little bit, you should get it real quick.

[Colin Gilchrist]

Also, under the Gap Settings, there are "gap methods", which control how Mastercam moves the tool in between each cutting pass. Change the option to 'smooth', and use the 'tangent line extension' to extend both sides of the path, along the direction of the cut. This allows the tool to extend past both sides of the surface, and may act as a substitute for the 'Direction' (surface lead in/out) button. 

[Leon82]

You can rough cut that whole part with optirough and up cuts and your depth step can be the bottom of the false bottom

So full depth cuts untill the profile is done, then the tool will go up to the chamfer and rough from the bottom up using the up cut step

 

You pick the whole model, then the outer rectangle as a machining area and cut from outside in. In steep shallow you can set depth limits. 

[killall-9]

Hi Guys,

 

Another question on this. I was succesful with the info shared here. Many thanks !

 

A knitpick question tho: I am writing another program with Surface Rough Contour op dripfeeding at 9600 baud :( is there a way i can have mastercam spit out R / I / K values for turning corners on my toolpath instead of lengthy xy coordinates ? or is this redundant 

[crazy^millman]

On 1/24/2019 at 11:22 AM, killall-9 said:

Hi Guys,

 

Another question on this. I was succesful with the info shared here. Many thanks !

 

A knitpick question tho: I am writing another program with Surface Rough Contour op dripfeeding at 9600 baud is there a way i can have mastercam spit out R / I / K values for turning corners on my toolpath instead of lengthy xy coordinates ? or is this redundant 

Look to your filter setting and go up to 95%.