Profiling question in Pro-Nc

[jeffroot]

I really think Pro NC rocks! BUT..........
I have run into a simple problem that is driving me CRAZY.

I have several parts I make that look like a domino with a corner radius on all edges. The last sequence in my 1st operation is a profile of the perimiter. I want to pick the verticle walls to define the profile......but i can't figure out how to get the toolpath to go deeper than the depth of the verticle wall and deeper than the corner that is between the verticle wall and the bottom edge.

Typically I like to cut profiles at least .01 into the spoil board.

I hope the solution is just a menu pick.........cutting deeper also helps when I use bull mills to do combination profiling and shallow surfacing.

ANY help is greatly appriciated.


Thanks,

Jeff Root

[JonasC]

hej,

well you can do it in a number of ways:

1. Put in a value in the AXIS_SHIFT parameter of the NCSequence. + is away from spindle. This will offset your entire toolpath by this amount. Of course your first slice will remove more material but in non steel or a small offfset it shouldnt be a problem.
This would be the easiest method.

2. Create a Mill surface that simply goes deeper than your actual part wall.
This would be the best and most controlled method.

3. Perhaps, I havent tried this, you can specify the OVERTRAVEL parameter and get the desired result.
And that would be the guess method....

Good luck, Jonas

[CAD/CAM Man]

I never thought about changing the "Overtravel" parameter, so I tried it, and the result looks like it only changes the start and end position along the X + Y axis.

Jonas, I typically use your method number 2.

BTW: You need to be very careful using "Axis Shift" because there are some cases where you can actually force the tool to gouge into the part.

I also agree that Pro/Nc is pretty good.

[jeffroot]

Jonas and CadCam Man,

Thanks for your replies.

I have used the axis off set for parts I made of aluminum. I manually over ride the feed rate to compensate a deeper than optimal first pass. I have also had a part gouge that really surprised me.

The part that started this thread is made of annealled 01 tool steel.
I ended up constructing a "dummy" part that had surfaces deeper than the actual part. A lot of extra work for a simple task.

My hope was that there was a way of entering in verticle over travel like I can for hole making........but I can't figure out how to do this.
Looks like it doesn't exist OR you guys would know about it.

I don't have experiance with other high end CAM programs.
NC has some strange quirks (check surfaces - why would anyone NOT want to check against the part instead of a surface) but I love the fact that eventually i can get it to make what I need. I have gotten so used to making toolpaths without a lot "dummy" models......that this one instance pisses me off everytime it pops up.........profiling parts with rounds on the bottom is the only time I have to make special models to to do a task that I feel should (could) be avoided with an over travel menu entry like we have with hole making.

All in all I'm a VERY happy with ProNC......I just can't figure out why I have never met someone in person who uses it.


Jeff Root

[CAD/CAM Man]

I've been using Pro/E since version 14. It has changed quite a bit in 15 years. Did you know that you can build manufacturing geometry directly into your manufacturing model without the need for a dummy part?

[jeffroot]

cadcam man,

Once again, I apperciate your help.

I am totally self taught and have large gaps in my NC knowledge.

I guess I was a little unclear........I should have said "dummy workpiece" not dummy model. I know about making workpiece geometry......is this what you are talking about?



Goofing around with the work piece model gets me confused sometimes....so I try to avoid it.......I have read somewhere that NC can output assembly (part?) models of the output of different sequences. I have never done this BUT think it is something I should look into.

Thanks,

Jeff Root

[JonasC]

Hej,

I get a little confused when you say workpiece geometry. Probably you are using the correct way to do it but it's called 'Mfg Geometry' in Pro/NC. This way any 'dummy' or 'help' geometry is being stored in your MFG model and it shows up in the model tree in the MFG. You COULD do it as a part of the workpiece also but thats complicating things. Anyway you find it under MFG SETUP and then MFG GEOMTERY, and it's basically a tool for defining mill volumes or mill surface (etc) that you are usingt in your NC sequences as a reference to what you are about top machine. But again you probably already are usiung them.

I have read somewhere that NC can output assembly (part?) models of the output of different sequences. I have never done this BUT think it is something I should look into

I'm not really sure of what you're talking about here.
First of all there is a possibility to have material removal based on a certain NC Sequence in the MFG file. This is done from the MACHINING menu and then MTRL REMOVE and then referencing the NC Sequence in question. This will basically give you an Assembly cut in the workpiece that's representing the material remove. There's a number of weaknesses (imho) with this function that keeps me from using it very often. They are:
1. This creates alot more references in your model that you need to keep track of. If you reference something thats part of such a removal this might complicate the model when doing changes later on.
2. The material removal representation isn't really that accurate. It does show stock allow(not always) but naturally not scallops or places where your tool is to big to access.

The other way you have of showing this is the option of using Vericut. I don't know how much you use vericut or NCCheck, but I tend to use NCCheck during the programming and then in the end I do a full check with Vericut. Reason being that I percieve NCCheck as faster (in most cases) but Vericut more accurate. Anyways, in Vericut you can export the cut model as an iges or step file. The only real use of this I've seen is when doing reverse engineering of really old programs that one doesn't really know what they do. Theese models are then used as templates to build a new part. If you're having 3d Surfaces that you 3D machine(in lack of better word) and you produce alot of fine scallops this export procedure is really cpu extensive and the end result isn't that good. However I've heard that CGTECH (Makers of veriicut) has put in some work here in recent versions but I havent tried it out for some time.

/Jonas