A simple question to anyone who has any idea what they're doing

[OOZ662]

Using Mastercam X2 MR2.

 

How do you tell Mastercam how large your "blank" is without it simply cutting the shape of the blank? Is that what check surfaces are?

[gcode]

see "Stock Setup" in the Machine Group

[JDowe]

If the part is irregular and roughed out

xform offset contour will give uniform stock around the otsiide - a bounding box will give

a rectangular or cylindical shape with margins

around the part

[Goldorak]

draw your blank in surfaces and save it as an .STL file

 

then use the STL as stoch in stock setup page

 

 

or simply create a solid if you have the option

[Thee Dragracer1951]

What porpose is defining stock in mill? I understand in lathe. That controls al of your rough cuts but does it work the same way in mill??? I've been using MC for years and never used stock setup in mills.

Might not be too old to learn new trix...

[Colin Gilchrist]

Jim,

 

In Mill, the stock setup function does two things for you. First you get to see a translucent display of the actual material, overlayed on top of your solid model. The second thing you get is it sets up the stock for Verify. You get two display options, wireframe and shaded. The shaded option also works with STL files to show you the material that is left over on your part after you rough it.

 

I love being able to display a translucent model of the material I just cut in Verify, on top of my part solid. It is still one of my favorite new features since CNC Software moved on from Version 9.

 

OZZ,

 

To answer your question about setting the "size" of the material for the toolpath, there are a couple methods. I'm assuming you have a solid model and you want to rough it out from a rectangular block. The method I use most often is Surface Rough Pocket. The Surface Rough Pocket method can be used two ways; to rough an actual pocket, or to rough out a positive shape from a block of material.

 

Surface Rough Pocket uses a set of surfaces and a containment boundary. The containment boundary "tells" mastercam what the size of the block of material (or top boundary of the cavity) is. You must put the boundary at the Z depth of the top of the actual block of material. Typically this would be a wireframe rectangle, but it can really be any closed 2D chain.

 

For other toolpaths, you would need to create and use a surface, typically called a "run-out" surface. Just create a rectangle with the surface creation option turned on, at the depth that you want to stop cutting at. This gives the toolpath algorythim an entity to "slice" and include in it's calculations. This would be used with parallel, contour, scallop, or Rest Roughing.

 

Check surfaces are surfaces that you want mastercam to NOT machine. They are used to keep a toolpath from gouging into adjacent surfaces that are not included in the drive geometry, but might be violated by the toolpath motion. Setting them as check gives you a way to not hit them.

 

HTH,

[cadcam]

Now are we talking about Lathe or mill for starters?

 

If we are talking about Mill are we talking about a casting blank or rectangle block you are cutting the shape out of?

 

As each thought has it's own option or options.

[OOZ662]

Sorry, this is Mill. Also, I'm cutting a flat surface with raised letters out of the corner of a rectangular prism sitting on its edge. I've been given the task of learning how to operate our three-axis mill with no background knowledge whatsoever and lack of time to read the Mastercam manual. I still don't understand how to chain anything but a containment boundary, meaning I only use Surface toolpaths.

[edmBosto]

quote:

---

Is that what check surfaces are?

---

Check surfaces will not be machined when selected in your surface toolpath.

It is a very good idea to verify your toolpath lettering. If the top of the letters is Z= 0.0

Then you should define your stock as Z with a positive dimenesion such as .005 at least. This way you'll see the skim cut in verify.

 

So when you set your stock ...

In stock origin in view coordinates on lower left set Z to .005, then in the dotted 3D view the Z should be set at a depth more than your machining on the toolpath. That's if top is your origin or Z 0 height.

Or you can create your stock by using the entities and expanding them by a certain distance.

I do that by going to the toolbar on top and click on create/ then bounding box.

 

Then in

[OOZ662]

My problem is that our bit has a cutting length of half an inch. When running a rough parallel toolpath, the first cut would sink the non-cutting portion of the bit about 1/5" in because it's cutting down to the top of the extruded letters even with the stock defined. How can I fix that?

[Colin Gilchrist]

In the Rough Parallel parameters there are two settings you need to use, Max stepdown and Cut Depths.

 

Start with Cut Depths. This dialog box tells Mastercam where to start cutting in Z and where to stop cutting in Z. Set the radio button to absolute. The Minimum depth is the Z height of your first cut. The Maximum depth is the Z height of your final cut.

 

Let's assume you are cutting your raised letters out of a 1" thick plate and the finish height of the letters is .3 thick. Z zero is the top of the material. I would set the Minimum depth to -.25 and Maximum depth to the height of the bottom of the letters, say -0.85.

 

Then you have Maximum stepdown. This determines what the depth of each cut is in Z. Say you set your Maximum stepdown to .25.

 

The first pass would be a -.25 in Z. The second would be at -.5, The third at -.75, ect.