Wireframe - ruled surface

[Brian Pallas]

Hello,

 

I have some parts to make and I am using the Wireframe Ruled toolpath.  There are basically three lines that are drafted outwards and have a radius at each corner.  I have the "across cut distance" set at .008 to get good definition on the rads.  But in the code, most of the cutting is just moving in a straight line, but it outputs the position every .008.  So there are just tons moves where only one axis just keeps moving.

 

 

 Is there a way to get MCAM to just output the end coordinate without all the stuff in between if only one axis is moving?

 

I am using X7 mill level 1.

 

For example - Instead of :  

 

X.8619

X.8554

X.8488

X.8423

X.8357

X.8292

X.8226

X.8161

X.8095

X.803

X.7965

X.7899

X.7834

X.7768

X.7703

X.7637

X.7572

X.7506

X.7441

 

We would just get:

X.8619

X.7441

 

Thanks,

Brian

[Thad]

I've never done it myself, but I think others have said that filtering your toolpath will eliminate those moves.

[brandon b]

There's a c hook for filtering.

 

I've tried it once or twice but couldn't figure it out.

[Teh Bear without Brains kinda idiot]

fILTERnci FilterNCI C-Hook

Use this C-Hook to apply Mastercam's toolpath filtering function to an external NCI file.

This is most useful for toolpaths that don't have the filtering feature as a standard option,

such as wireframe toolpaths.

 

After opening the C-Hook, Mastercam prompts you to select the NCI file.

 

The Filter settings dialog box displays. Enter the filter settings and click OK.

 

Mastercam prompts you for a name for the modified NCI file.

 

Once you have saved the filtered NCI file, you can import it into your current part file.

Typically, you will need to do this in order to post it. If the original operation is also

in the current file, you might wish to disable posting for it.

 

yOU CAN MAKE nci FILE While posting

When you post an operation, you have the option to create and save a text NCI file. This contains the information from the binary NCI file in a text format so you can read it. Use the control definition to tell Mastercam how you want to work with NCI files. Consult your Mastercam reseller if you need more documentation.

[Brian Pallas]

Thanks for the replies.  I ran the filter and that reduced the code a lot.  We're going t0 run these parts this afternoon and we'll see how it goes.  

 

After I imported the filtered NCI file back into MasterCam and used it as an operation on the stock model, the stock model was showing that the filtered path was going to cut quite a bit to much.  Looking at it in backplot though, it looks good, and the numbers were matching up with the unfiltered operation.  So I am not sure what is going on with that.  We will see what happens at the machine, hopefully I am not overlooking something.

[CJep]

Another solution would be to use the McamX9 software, mill1 & mill2 have been combined, you would have access to some of the surface tpaths.

[Brian Pallas]

Yes, the filter worked well.  It got rid of 97% of the program, and the tool ran well.  Thanks for the tip.