What's new
What's new

FeatureCam Post for a Brother C-00 CNC control

rfrink

Cast Iron
Joined
Nov 21, 2005
Location
Ohio
We have new Brother machines and new to FeatureCam...so I'm knee deep in a steep learning curve right now.

I'm struggling with Cutter Comp. I don't like to use it and normally don't for the stuff that we do. But my Feature Cam NC outputs have it in there.

The Controller is a Brother C-00....and the post processor that I have is for a Brother TC-31A.

Even if I have "enable cutter comp" unselected in the Featurecam Options-milling screen.....the NC file has a G41.

See the following code:

( ROUGH1 BOSS BOSS2 )
M400
M8
G99 G41 D1 G0 X1.0559 Y-0.3159
Z0.2
G1 Z-0.2 F75.0
X1.0493 Y-0.3124 F150.0
G3 X1.0 Y-0.3 I-0.0493 J-0.0918
....


The coordinates are the left side of the endmill. I really want code written as endmill centerline paths and no comp.

This post processor doesn't insert a G40 anywhere ....so I'm thinking that something is wrong....

Do you know if there is a C-00 post processor?

I have a phone call into the sales guy...and waiting.

thoughts?

Rob
 
Yes there is a problem with the post. The G41 D1 codes should not be on the G0 positioning line. They shouldn't be in the program at all since you unselected 'Enable Cutter Comp'. Another issue is no G40 to turn off cutter comp which would be necessary if you were using it. That being said I usually program with cutter comp set to 'Wear' (I haven't used FeatureCam) to allow for some adjustment to the tool path while running. The G41 needs to be on a G1 X, G1 Y or G1 XY move to function if you want to use cutter comp.
 
Rob,

Which Brother machine do you have? Depending on your response, I may be able to comment further or provide a copy of our post that could be useful. BTW, is you current post using the G100 tool change cycle?

Fred
 
I'm struggling with Cutter Comp. I don't like to use it and normally don't for the stuff that we do. But my Feature Cam NC outputs have it in there.


Even if I have "enable cutter comp" unselected in the Featurecam Options-milling screen.....the NC file has a G41.


Rob

While I may not understand why you don't want to use cutter comp ( nor am I going to advocate for or against it ), you should look into:
Machining Attributes -> Milling.
There you'll find a setting: Finish Cutter Comp.
If you uncheck it, there will be no comp of any kind will be output.

The way it works is:
Finish cutter comp = OFF -> No G41 or G42 is output
Finish Cutter Comp = ON - AND - Partline program = OFF -> Wear comp ( G41 or G42 is output, toolpath uses centerline )
Finish cutter Comp = ON - AND - Partline program = ON -> Full dia comp ( G41 or G42 is output, toolpath uses tool edge = exact part geometry )
Finish Cutter Comp = ON - AND - Partline program = ON - AND - Rough cutter comp = ON -> Both, rough and finish operations use Full dia. compensation ( same as above, but applies to both Rough and finish )

Basically, the usage of cutter comp is independent of the post selected, rather it is controlled by your preference for the part on hand.
IOW you may create the program for just about any machine, regardless whether it is capable of full cutter compensation, limited cutter compensation, or not at all.
 
If there is no other G4x anywhere in your posted code, there's a good chance that G41 is hard coded in the post, and that the actual code IS centreline.

Look in the program start/tool change/segment start formats in your post and see if G41 is explicitly written anywhere in there. If it's not, but it does have <COMP-STAT> then you are still outputting comp'd paths as per Seymour's explanation above.
 
Rob,

In addition to my previous question regarding the Brother model, can you tell us the version of Featurecam you are using (usually a year like 2016)?

I looked at the standard Brother TC-31A post...it has obvious errors in the Program Start format. Namely, it has hardcoded G99 and G41. Both need to be stricken from the format and replaced with a <MOTION> reserved word.

In the case of the G99 I don't understand this at all. I associate G99 only with cycles and return to R plane - normally never hardcoded. Likewise G41/42 is usually not hardcoded, but is introduced with <COMP-STAT> and <COMP_START> in the Linear Move format. Also, you need to introduce the D word on same line with some additional logic in the post.

That is a long winded way of saying your post needs some work. The main reason for asking about Featurecam version is that this influences how easy it is to provide info on what to change in your post or to provide you with a post that has most significant edits already done.

Fred
 








 
Back
Top