Cut depth, Gap setting, Advanced setting questions

[nickelback]

How do you know what to change the Cut depth, Gap setting and Advanced settings to when doing 3D surface machining. I have gone through different tutorials and they tell you what to put in the boxes, but what does the stuff mean? Why do you change to certain settings for certain paths? Is there any info that explains this in depth more than the ? info from the software? Thank you for any help.

[Thad]

Help is always a good place to start. In most, if not all dialog boxes, there is a question mark icon. Click it to open up context sensitive help. In the help window, there is usually a "Field Definitions" tab that will give a description of each field.

 

Cut depths is when you want to specify what Z level to start cutting at and where to end. You can use this to help contain your toolpath. You have the choice of absolute or incremental dimensions. Absolute dimensions are exactly that and incremental are from the surfaces that are selected. For example, any detail that has 3D form on it, we leave the height of it heavy, as the true height will get finished at 3D. Maybe the part will really finish at 3.5 tall, but the actualy piece of steel that I have is 3.75 tall. If I use incremental cut depth, the first pass will be at 3.5. Ouch! If I use absolute, I can specify to start cutting at Z3.75. And just to make sure that I don't cut my vise, I can set my max cut to Z1.0. The toolpath won't go below that Z depth, even if the surfaces and containment boundary would allow it.

 

Gap settings were explained very well in V9 help, but I haven't looked them up in X yet. The gap settings dialog box confused me for a long time. It never made sense to me until I read the help. Think of a parallel toolpath how it goes back and forth. Between those 2 passes, the toolpath has to get from the end of one pass to the start of the next. That's called the gap and gap settings control the movement. The dialog box says "if gap is less than"...use the method set in the drop down box. Broken, smooth, follow surfaces, and direct are the options. Help should show you these movements. The gap size defaults to 300% of your step over. So if you stepover .100 and the gap is less than .300 (it could be more, based on geometry), MC needs to know how to move the tool to the start point of the next pass. If it exceeds .300, then the tool will retract in the Z axis and then rapid to the next pass start point. If you get a lot of retracts (common with 45 degree machining angle), you can change the gap to a distance (say 6 inches), instead of % and that will keep the tool down into the part. Sometimes this produces undesireable results, so make sure you backplot it.

 

The advanced settings, I've only change the default to "only between surfaces." I can't put that into words so you'll have to read up on that one.

 

Thad

[nickelback]

Thank you, Thad!! Very helpful to me!!

[Thad]

 

Thad

[nickelback]

Good!! I just purchased the Mastercam X Mill Tutorial from In House Solutions. This is a very in depth book. It explains what everything is very well. I have never found a book as good as this one.

[Thad]

Check out the Mastercam Handbooks by our very own Charles Davis, from San Diego CADCAM. They're the best books that I've seen.

 

Thad