Problems cutting filled engraving.

[ckirchen]

Often, our customers will give us a 2D vector artwork, which we bring into ProE and add to their model as a sketch.


For example, a customer wants us to add text (about 500 characters) and a complex logo to amold insert. I'll add the artwork to the model and switch to ProNC for machining. The engraving sequence will engrave along a path, but that doesn't work because the text and the logo need to be filled, so I can't use the sketch feature directly. The two ways I got it to work are:


1. Use the sketch to create an extruded cut. Then createa milling volume around the artwork, to the same depth, and use trim so that the volume is just the artwork. Next use a volume sequence to do the milling.


2. Use the sketch to create an extruded cut. Then createa milling window around the artwork, to the same depth. Next use a volume sequence to do the milling.


Both methods work; my problems is that the calculation time for the volume sequence in both cases is long. The part I did yesterday hadabout 30 characters and it took almost 10 minutes to calculate the toolpath. I have a $150 CAM package that will calculate thesame toolpath in less thana second, but I would like to keep it all in ProE.


The other issue I have is that I don't like that I need tocreate a cut out of the sketch to proceed. Adding the cut to the model greatly increases it size because of all the little surfaces that make up the sides of the letter.


What is the best way to machine filled text and artwork in ProNC?

 

[Guest]

Have you tried creating a 'cosmetic groove' and use engraving?

 

[ToolDude]

ckirchen,


once you get the volume built I would cut using a type 3 surface milling sequence with a reasonable step over an depth of cut. only select the bottom surface of the letter or text if you need the walls of the text drafted i would use a tapered cutter. You don't say whether you are on a flat surface or need tapered text walls.

 

[kkar]

Use cosmetic groove and then engraving put don't forget to use points only is mfg setup.

 

[ckirchen]

Kent and kkar, I had a chance to try out using cosmetic groove, and unless I'm using it wrong, it only generates a tool path that follow the cosmetic groove, not the area contained by the groove.


ToolDude, Type 3 Volume milling is exactly what I used to get the job done. But there has to be a better way! As I mentioned above, the toolpath takes forever to calculate (coffee break) and the presence of extruded text on the model slows things down.


Any other tips?


Thanks again, Chris

 

[ToolDude]

CKirchen,


What you said is correct in your post cosmetic groove will only follow the groove not the area contained by the groove.


what I find that slows down the tool path generation is usually the wayparameters are set for cutting the volume. If possible set the sequence tolerance and step over and step down as loose as possible to speed tool path generation. if the wall finish is a problem try using pocketing which makes a profile pass on thewalls to finish them.

 

[ckirchen]

The job that I was working on when I first posted was engraving with a .0313" ball mill; at that size, tolerance, step over and step down are all pretty tight.


Wall finish is not a problem; the finished part looks great!


I compared the estimated run time of the ProNC gcode, the actual run time of the ProNCgcode, andthe estimated run time of the SheetCAM gcode; they were all very close. It seems like ProNC and SheetCAM do the same thing, ProNC just takes a lot longer to get there.


For now, I will do any filled engraving with SheetCAM.


Thanks for all your help, Chris