MCX depth cuts question

[charper]

Why is it when you choose the depth of your engraving you have the option to choose absolute or incremental depth when REGARDLESS of what you choose, you can always mark the option on the same page to make depth cuts of a maximum value?

[tobyaxis]

I'm not an MC Guru but it leaves the option to use Incremental depths. Also the Tool Retract position set Incrementally allows for shorter cycle times because the tool doesn't fully retract above the part.

Is this what you mean, or am I as lost as you? LOL

[Matt Berube]

I may be way off here as well since I do not have the engraving option...

Are you aware of how the incremental choice affects other Mastercam toolpaths ?

Lets say I have a bunch of contours to mill but they all lie at different "Z" heights. As long as the geometry is at the actual height I want to cut I can chain them all and use incremental depth of "0" and they will all be cut at the proper heights.

If you're not working with 3-D wireframe or solid models it is unlikely that you'd use the incremental choice.

Does this help at all ?

[charper]

Thanks guys.....I think I am getting there... I just ran a one tool path engraving with my students of their names in wood. I put the depth as absolute and made depth cuts into the wood.

If I wanted to do each initial at a different depth, I could conceivably chain them together. Suppose I wanted the "C" at 1/4" and the H at 1/2" the "H" would be incremental from where the C finished off? Therefore the depth of the C would be -1/4" absolute and the depth of the "H" could also be -1/4" but incremental from the "C" and the overall effect would be a "C" at 1/4" and an "H" at 1/2" or am I way off?

So the second tool path is incremental from where the first tool path finished? and not from the home position? Thus allowing for the tool to not have to retract all the way to the home for each tool path. I could see using this, if I can figure it out

Or am I beyond hope?

[Matt Berube]

You are not beyond hope but you don't quite get it yet...

It has nothing to do with where the toolpath finished.

Using your example, lets say that your letter "C" is at a height of zero and lets say your "H" is at Z-.1

If you toolpath these items using an incremental depth of -.005, your "C" will be cut at Z-.005 and your "H" will be cut at Z-.105

I am thinking of how to explain it better...

I assume your "C" and "H" are at the same height. To change it to the way my example works, use XFORM, TRANSLATE and move the "H" Z-.1

Now your letters are at different heights and you'll see what happens if you create a toolpath with an incremental depth and backplot it.

Hope this helps.

[tobyaxis]

Originally Posted by charper Or am I beyond hope?

If your trying, and learning....Your Not Beyond Hope

[Mike Mattera]

Absolute is in relation to the Absolute Zero. Incremental is in relation to the actual geometry you selected. 99.99% of the time your geometry is at the top of the part (Z0) so you wont see ant difference. If you Geo is Z-.5 and your Depth is Incr -.5 , Your NC output will be Absolute Z-1.

Mike Mattera

[Mike Mattera]

(after thought)....

It's handy when your selecting arcs at different heights and you want them all drilled some distance from their respective surface (i.e. Tapping Z-.65). Using an Incremental Tap depth on an assortment of different arcs, at different Z heights wil do this for you. A great option is it's used right.

Most people are afraid if the Incr option because they think it will change their NC output to G91 (incremental). Not So.

Mike Mattera