Some basic machining & programming questions

[Diedesigner]

Hi all,

I have some 3D machining & misc questions. I am running v8.1

 

-- If I program relatively shallow contoured surfaces with a flat end mill, or a “bull” mill, will MC’s output produce an accurate contoured surface? I am thinking of using pencil tracing to remove the material that was missed in the inside radii or fillets.

 

-- This question arises from my lack of knowledge in multi-plane programming: Is it possible to program multiple faces of a block where each face will be run as a separate set-up on my VMC? Right now, I rotate my block around and re-save the file with a different file name for each face I need to program. If it is possible (and I strongly suspect it is), how do I display the face I’m working on so that it shows as the “top” surface in “Verify”, the same way it will be sitting on my VMC?

 

-- Can I “hide” tool paths on different layers, so that face #1 is programmed on layer 1, face #2 is programmed on layer2, etc?

 

As always, any help you may give me is greatly appreciated.

 

Chris

[Brendan P]

You need to go into tool parameters tab and

click on T/C plane button.

Inside this dialogue you can assign your specific

tool plane/const. plane/wcs, for which ever

side of the "block" you want to machine.

This is how I do it.There may be other ways that

I don't know of. It takes some practice.

I do not think that you can put your "toolpath"

on different layers,because I dont think that they lie on any particular layer.

I think that they are part of the nci file.

Please correct me if I am wrong someone.

However, by hitting ALT+T you can "hide" them.

 

 

[Tony]

Chris

I could give you a crash course on Mcam.

I am next to the Dupage Airport.

A Saturday morning would work.

 

Tony

 

[ 02-22-2003, 12:59 AM: Message edited by: Tony ]

[jadaro]

I've been running tool paths across NURBS surfaces, i rough cut with a flat endmill telling it to leave a little bit of stock, then i finishing pass the contours with a ball nose endmill.

 

If your machine accepts (G54)Coordinate offset (which it should, ), then you can have several different COPIES of the same file, each with different tool paths-- As long as you don't change any tool height offsets, or change the G54 offsets, the the programs should pick up where they left off last. This is something i have to do with our Amera-Seiki as it has no DNC cache.

 

For a better example:

You could run all your roughing passes in one copy of a program, then without changing the setup on the machine, run all of youy finishing passes with two or more other programs. The only reason I would see to do this is because you have no ability to do DNC and your machines won't hold the program in memory because they're to large. This may not be very conventional, but tis the only way we can do it right now, as our school is broke.

 

When i say copies, i mean that there are different copies of programs all containing identical geometry, but the tool paths are different for each machine.

[stonker]

There is a nice WCS tutorial on the mastercam website I have just started. I think it is just the thing you need. I create new toolpath groups to seperate toolpaths. I hope I understood your question and this helps.

[Rick Damiani]

quote:

---

-- If I program relatively shallow contoured surfaces with a flat end mill, or a “bull” mill, will MC’s output produce an accurate contoured surface? I am thinking of using pencil tracing to remove the material that was missed in the inside radii or fillets.

---

On a shallow surface with a flat mill you will get some steps in the surface. With a bull or ball mill and a small enough stepover you will get a smoother surface. I'd sugust using surface|finish|shallow in this sort of situaiton to get the best finish.

 

quote:

---

-- This question arises from my lack of knowledge in multi-plane programming: Is it possible to program multiple faces of a block where each face will be run as a separate set-up on my VMC? Right now, I rotate my block around and re-save the file with a different file name for each face I need to program. If it is possible (and I strongly suspect it is), how do I display the face I’m working on so that it shows as the “top” surface in “Verify”, the same way it will be sitting on my VMC?

---

Yes. Use the T/C button in the toolpath parameters to assign a new tool and construciton plane to the toolpath, and change the work offset value. In MasterCAM workoffsets are numbered from 0, with 0 being the first work offset your post supports, 1 being the second, and so on. -1 uses the default offset, whatever that happens to be.

 

quote:

---

-- Can I “hide” tool paths on different layers, so that face #1 is programmed on layer 1, face #2 is programmed on layer2, etc?

---

No. What you can do is toggle the toolpath display off by pressing ALT-T on the keyboard.

[jadaro]

Why didn't I think of that before...

 

You can post individual toolpaths by selecting the one toolpath, and then selecting POST on the operations menue.

 

You can selct a toolpath group, or you can slect two or more idividual paths, by click on, then holding down control and selecting the others.

[Rick Damiani]

quote:

---

You can post individual toolpaths by selecting the one toolpath, and then selecting POST on the operations menue.

 

You can selct a toolpath group, or you can slect two or more idividual paths, by click on, then holding down control and selecting the others

---

Be careful of doing this without carefully checking the code that is generated. In some curcumstances with some posts things may not work as you expect them to. Subprogram numbering can be particularly troublesome.

[Bill Cronkhite]

Thanks for the tip on ALT T. I've been changing a parameter on my roughing passes to get those out of the way so I could see to create my finish work. Spent 4 years in UniGraphics, but learning MasterCam on my own.

[Guest CNC Apps Guy 1]

and if you're in the operations Manager, if an operation is selected, you can press "T" and that toolpath will not be visible as well.

[Rick Damiani]

quote:

---

and if you're in the operations Manager, if an operation is selected, you can press "T" and that toolpath will not be visible as well.

---

While we are trading tips...

 

You can also select the toolpaths you want to turn off (use control or click on the group if you are using groups), right click, and select 'Options' from the menu, then select 'Toolpath Display' and set them to on or off.