Open Pockets

[slideleft]

Hi All,
Fairly regularly I make parts that for lack of a better term I call "open pocket". They are parts that need to step down incrimentally in Z, cut past the edge in some parts, and cut to an edge in others (iges file attached). I cannot find an easy way to do this. The closest I have come is "finish shallow" toolpath, but this will not let you cut in z-steps, only a final depth. I can fake it in "rough contour", but this only works if you program in exact "absolute" depth you are cutting to. If I have several face depths, I have to have seperate routines. Incremental always gives me the dreaded "no cut found, check...". This seems like it shouldn't be so hard. Any ideas?

Thanks in advance,
Jeff

[slideleft]

[txcncman]

Why don't you create some geometry and build some containment lines and use pocketing? I guess I have found compared to programming with a note pad and a calculator, nothing using MasterCAM is hard.

[metlshpr]

From what I can see this is a 2d part. Why are you using 3d paths? Just like TX said, create some geometry, ie edge curves and outside pockets, and do 2d pocket routines. I would use dynamic core milling and contour the edges to finish. Its pretty simple if you approach it this way.

[slideleft]

You guys are right. It is a very easy part, 2D for sure. But.... I have many more similar parts (nested together) where this came from- well over a hundred variations on a theme, with new ones coming each week. To create extra geometry for each part does not seem practical.
BobCAD (of which I am no big fan) has an open pocket routine where you use solid lines for the edges you must stay inside, and dashed lines deliniating the edges you can spill over (you get to say how much). Mastercam usually can do anything BobCAD can do so...??? Any other ideas?
Thanks,
Jeff

Mastercam X

[txcncman]

Since you did not upload a sample file, when I get time, I will try to create something similar to your picture and show a couple of different ways to program it.

[slideleft]

Here is an iges of a Semi typical job of parts nested. I will do 2 plates of these using G54 and G55. Material is usually about .375x3x20" Al, SS or Ti. This set of parts will be machined with 1/4" carbide endmills, 1 rough, 1 finish. Op 1- drill holes and mill reliefs, Op 2- bolt to tooling plate and cut around the profile.
I REALLY appreciate all help on this. I've done so much more complex projects easily with Mastercam. That the easy ones should trip me up is really frustrating.
Jeff

[txcncman]

Just getting back to messing around with this.

Method 1

Step 1 - Make new layer and create bounding box
Step 2 - Make new layer and create stock
Step 3 - Make copy of Top WCS (Rename to G54), Put origin on corner of stock, Set G54 WCS as active for Cplan and Tplan
Step 4 - In Operations Manager - Stock Set Up - Set stock
Step 5 - Make new layer and create curves on edges as needed
Step 6 - Make new layer and project (copy) curves to same Z
Step 7 - Make new layer and offset contours / curves to make pockets / islands
Step 8 - Use Toolpath - Pocket to face to needed Z levels
Step 9 - Machine contours

Time on task - less than 1 hour

[cadcam]

you are making the part from a plate corect if so you have the main boundry and the part a simple pocket with facing and a contour .

[txcncman]

This one is kinda dirty. I could have taken more time on extending the surfaces.

Method 2

Step 1 - Make new layer and create bounding box
Step 2 - Make new layer and create stock
Step 3 - Make copy of Top WCS (Rename to G54), Put origin on corner of stock, Set G54 WCS as active for Cplan and Tplan
Step 4 - In Operations Manager - Stock Set Up - Set stock
Step 5 - Make new layer and copy surfaces
Step 6 - Extend edges of surfaces for facing
Step 7 - Use Toolpath Surface Finish - Flowline - be sure to select check surfaces
Step 8 - Toolpath - Contour to clean up and cut depth

Time on task - less than one hour

[cadcam]

txcncman, what version are you guys using so when I do mind you guys can open them. I see X4 or ealer due to the MCX.
I have on this box X3,X4,X5,X6... thanks guys

[txcncman]

I am on X3 here. Sorry if that was not mentioned before. Have used 9, X4, and X5 all within the last year depending on my work location.