I am currently working on a project for a customer that is a simple 5-axis part and can't get passed the 3 axis floor operations. To say my frustration level is high would be a gross understatement hence the following sarcasm.
Issues I have run into so far:
1. Cannot select multiple floors in a single operation and get single paths on each floor. Why not? Using Floor Wall results in 5 or more depth cuts near the floor instead of 1. Why?
2 . The NX tutorial for a 5-axis part returns an Alert "All Cut Area faces must belong to the Part Geometry". Really?! I'm using your supplied tutorial and following each click.
3. There is an obvious bug in Engage settings when selecting open and closed area boundaries in the same operation. If you set closed area engage to ramp on shape then set open area to linear - relative to cut the path result is closed areas are the same as open. This is NX 10 and no one has brought this up? Are you guys so conditioned to the mind numbing amount of dialog boxes and clicks that when you do get a result that won't gouge the part you're so excited you forget what it took to get the still inefficient result?
So the "solution" to items 1 and 3 above are to create an operation for each pocket floor and open and closed profiles? Oh goodie! I can't wait to get the project where I will have 200+ pockets that I get the pleasure of selecting these individually. Fun times.
Need to change to convex hull
Need to change to follow instead of cut
*See image attached*
2. NX works with a workpiece structure. If you have a workpiece selected you cant click on faces that arent in the workpiece.
If you dont put an operation under a workpiece you can select your workpiece and cut area in that operation
3. Not sure what you mean?
Post a file
4. Some Floor or Wall geometry may not be cut because of Tool Overhang.
Cut Parameters > Containment > Overhang
5.Some regions were ignored because they are too small to engage.
Reducing the Minimum Ramp Length for engages or turning on Minimize Number of Engages can reduce these.
Non cutting moves > closed areas > Engangement size or length
Your tool is too big to ramp into the pocket with your stock and engagement settings
You sound like a guy who just switched to NX with no training and is just pissed off in general LOL>
If you post a file I'm more than happy to send back with what you ask later tonight.
LOL, Not pissed in general, just with NX. Yes you are correct, training consists of Learning Advantage and trial & much error, haven't used NX since 7.5 but not enough has changed for that to be a reason. I am too used to a much different workflow that requires much less effort so when the simple things like this require so much input...
I appreciate the response. I am working through what you listed and will let you know. Due to customer restrictions I cannot post the file I am working but will find another file to post containing the issues I'm having.
It's just a matter of me understanding what NX needs.
NX is all about setting up template files so you dont have to do the same settings every time.
You can make you own custom ones too.
I rarely run into any things like you described but I've spent a few hours setting all the defaults.
Below is a video of item 3 on my whine list.
The operation has 2 closed and 4 open areas. I start by generating the operation with open areas "same as closed" but what I need is open areas to be "linear - relative to cut" and closed "ramp on shape" to avoid geometry not shown. What am i missing? This looks like a bug to me.
The cut pattern detemines closed or open area's, not if the boundaries are open or closed. Because you are using a profile path, all area's are open -even the closed boundaries-
In the non cutting moves this is also indicated by the tooltip pictures
If you cut a pocket with a follow periphery pattern and select Add finish pass, then you can see the interpretation of open/closed area non-cutting moves.
I agree that this may seem confusing at first, but once you know that it's depents on the cut pattern, it makes sense.
You will have to create 2 operations to achive what you want.
1. Select all closed boundaries and set non-cutting-moves open area to same as closed
2. Select all open boundaries and set non-cutting-moves open area to liniar relative to cut
In my opinion it should not matter whether NX or the user identifies the open or closed profiles. The system can obviously handle the difference between open and closed in the same operation. So I conclude that it should honor my mixed selection of open and closed profiles in the same operation.
In my opinion it's broken. When the profiles are selected I have to tell NX Open or Closed. Ok NX then follow the engage parameters entered.
I'll file an IR but since my percerption is that the majority of users find the extra clicks acceptable I doubt it will go anywhere. But I'll try.
Thank you for the response.
What exactly are you trying to do? If you use a smart toolpath and give NX your check geometry you have extra options when the tool is "against check" which seems what you want to do...
Every CAM programmer searches for perfect software that doesnt exist. 1 extra operation to completely fine tune your program is such a big deal?