Creating a model from G-code

[Guyinthedesert]

I'm just wondering if there's an easy way to do this. We have a family of parts that have been in production for several years. They were originally programmed by our customer, so I don't have access to any source files, models, etc. All I have are the paper blueprints. What I'm trying to do is to update the toolpaths to take advantage of Opti-core and Opti-rest to speed things up, smooth things out, and eliminate a lot of air cuts.

 

When I began drawing up a model for the first part, I soon discovered the drawing is riddled with errors, missing dimensions. There are also many programming errors that seem to have never been caught by inspection. So now, what I need to do is draw my model to match the parts we've been making, right, wrong, or otherwise.

 

I managed to draw out one contour from the G-code entering points from the program, then I had to calculate all the arc centers. Took way too much time, and way too easy to make a mistake. I know I can use Vericut to generate a STL from the G-code, but an STL doesn't help me with generating toolpaths. Anyone know of any way to generate either a model, or even just 2-d geometry?

 

TIA

[Guest]

Best thing to do is just start fresh.

 

Cimco can save your geometry as a DXF but you'll have a ton to clean up.

 

AFAIK, there just sis NOT a reliable to do this.

 

Were it me, I'd just start in and get done

 

JM2C YMMV

[JAMMAN]

I'd start with a finished part and cmm/calipers/mic/height gage whatever it takes at whatever skill level you have available. Back in the 7 days you could rpost and backplot with MC, save geometry and offset for tool if necessary. Don't know if that is available in the X series.

[Guest]

Back in the 7 days you could rpost and backplot with MC, save geometry and offset for tool if necessary. Don't know if that is available in the X series.

 

It is not, it went away after V9

[Newbeeee™]

NCPlot would help you 'tune' the code (it's a backplotter) to take out air cuts.

 

Having never used vericut, you say it can produce a stl from the gcode? Can you not then import the stl into mcam and go from there?

 

On similar (old) stuff we have re-done to make use of the new paths, we have effectively optiroughed and posted that bit of code only, and pasted that into the original program so all the finishing etc is as was.

Last thing you want is the customer getting something slightly different to previous...

[Guyinthedesert]

We had one computer that still has V9 on it. I tried running rpfan, but I couldn't get it to work.

 

 

I wasn't aware that I could select an STL for my drive surfaces with Optirough. Is this new? I just tried it and it worked great. That solved my problem for the roughing ops. Thanks all

[JAMMAN]

I had problems with it too and ended up on the phone with Jay Kramer who walked me through it. It's been since V8 was first released.

 

The rpost is probably looking for clues in the NC code that it was posted with a fanuc post, I'm sure it is as simple as adding a couple lines of code to the header or footer. Anyone have recent experience with this?

[Newbeeee™]

I did a quick search and there is a STL to step converter available.

I don't know how good it is or of any others (stl to sat or parasolid or iges etc) available.

Anyone using any?

[Jeremy Herron@DBS Solutions™]

I have tried several of the free ones, but not with any sucess. The step files ended huge or unrecognizable by mastercam. Could have just been me though, I did ot have much time to mess with it.

[mkd]

have you thought about contacting the customer for the original CAD/CAM files?

 

if you can get to an STL from MC RPfan/Vericut or scanning finished part i believe GeoMagic can clean it up into a simple solid.

 

of course vericut can export cut stock in IGES and STEP format (among others).

[Dave Ball]

Solidworks with DezignWorks plugin and a Faro arm would be my prefered method.

[gcode]

At a previous job I once got about 50 customer supplied Fanuc NC files for a series of parts we were bulding.

 

Naturally, the bose wanted to run them on an big gantry mill with an old Allen Bradley control

 

I ran them through Predator VCNC and saved the output as NCI, then ran the NCI through our AB post.

 

The milling output was perfect, but the drilling cycles took a little tweaking.

 

I could have backplot the NCI and saved it as geometry, but that wouldn't have been much use building a model

 

as the NCI was C/L of the tool , not the shape of the part.