Verifying a facing op

[poconnor]

Hey All,

I'm having trouble viewing a facemilling operation with 'Verify' viewer. I know the operation is taking place but it doesn't show up when I preview the program. I'm flycutting a 2.5" path on a sheet of plastic on a Router program. Any ideas would be appreciated.

[Guest CNC Apps Guy 1]

Have you set up your material in Job Setup?

[Matthew]

If your stock origin is set to z=.000 then there is no material to be removed.

 

You could try setting your stock origin to

-.010" or +.010". This should allow .010" to be removed in the verify.

 

Hope this helps.

[poconnor]

My material is set-up and all the other operations show-up. I'm milling the slot 1/8" deep in 1/2" mat'l. Everything seems to check out all right. The facemilling shows up when I backplot just not in the 'Verify' mode!...Could this be a video card problem???

[Keith Graydon]

hi po,

all of the ^above^ plus

 

switch to front view in mastercam before pressing the start button in verify. you may then see where is space your tool might be. just to be sure, also check the pluz/minus value of the flycutter in mastercam. be sure that is is set to what u want. easy to miss a - sign.

 

 

-klg

[steve f]

poconnor,

 

I had this problem in v8.1.1 as well. Either it wouldn't show anything being machined or the facemill would take 1/4" in verify when I had only specified a .01 or .02 depth of cut. Maybe a video card problem?

 

Steve

[poconnor]

I've checked everything and it all checks out ok, so I'm just gonna assume it's related to the video card for now. Waiting to here back from MasterCam. Thanks for the help guys!

[Keith Graydon]

how did you define your tool? I use "slot mill" definition for a flycutter. not a custom tool.

 

 

-klg

 

[ 02-27-2003, 03:11 PM: Message edited by: Keith L. Graydon ]

[poconnor]

It must be video card related. When I take off TrueSolid mode the tool and path show up fine.

Thanks for the help guys!!

[Jack Mitchell]

poconner,

 

Guaranteed, this anomaly is not the video card.

 

Verify is accurate, bet your life one it - it's only math wearing shades don't you know!

 

Upload this to the ftp and the members will solve this problem.

 

Regards, Jack

[PE @ IHS]

Make sure that the facemill has been defined properly. Right click on the tool in the tool parameters page. On the right side of the screen you should see a 2D outline of the tool shape. If you see an X, it means that the tool has not been defined properly, and MC doesn't know how to show it during verification.

 

Since the tool dia is defined, your toolpath is correct, but Verify also needs tool lengths, flute length, and in the case of facemills you also need to enter corner radii/angles.

 

Peter Eigler

[Surface]

While we are on the subject of face milling, I have a question which I have yet to figure out. Toolpaths/face; Is there any way to make the cutter climb mill? Say I have a 1 inch wide, which I want to face with a 3/4 endmill. I want to climb mill both edges to minimize the burr. Just one pass in each direction.

[cadcam]

Surface you have the option in Faceing to go one way so that you could have it climb cut alwas.

 

Look under cutting method.

[Surface]

I did see that option, but that's not really what I was looking for. My problem with this particlar toolpath function is that the first cut is always conventional milling.

[cadcam]

poconnor Check two thoughts that happen to my students all the time.

 

1. look in the Define Tool this were the info for the tool is.

Under the first Tab check and make sure the at the bottom were it says Profile it is set for Auto.

 

2. In Job Setup were it says Stock Oragin add say .05 in the Z value so the stock box will be a little above your part on the screen.

 

Now give this a try.

 

[ 02-28-2003, 10:53 AM: Message edited by: cadcam ]

[cadcam]

So surface what you want is it to 1st cut climb on the left then pickup and climb on starting say from the top on the right?

[poconnor]

Well CadCam,

 

What can I say after 3 days of messing around with this problem you solved it for me in 5 seconds. Sometimes things are so simple you can't see them staring you in the face. Thanks to everyone for their help. I had the profile set to custom and as soon as I changed it to Auto it worked like a charm. Thanks again to all of you guys!

[Keith Graydon]

Glad your fixed Po.

Not to steal jays thunder but i think james nailed this one first.

 

quote:

---

Have you set up your material in Job Setup?

---

followed closley by Matthew

quote:

---

You could try setting your stock origin to

-.010" or +.010". This should allow .010" to be removed in the verify.

---

 

[ 02-28-2003, 11:24 AM: Message edited by: Keith L. Graydon ]

[Surface]

Not exactly Jay, I want to start at the top left, mill x+, then y-, and then x-

[cadcam]

Surface you are right at this time I can not make it happen the way you state.

[Rick Damiani]

quote:

---

Not exactly Jay, I want to start at the top left, mill x+, then y-, and then x-

---

There is a slightly non-obvious way to do it. Use a pocket toolpath and set the pocket method to 'Facing'. Be sure to turn off the finish path, as it is kinda pointless. You don't get the high-speed loop option from the Facing toolpath, but it dosen't sound like that's what you want to do anyway.

[cadcam]

Hey rick forgot about that. I just went with the basic Facing and forgot about that one.

[Fred from Université de Sherbrooke]

An other way would be to do your facing toolpath and reverse it.

Worked fine for me.