Any UG programmers?

I've been using UG since V15, and wondered if there are any others on this board that use it.

I mostly use it for 3 axis work, and the occasional horizontal/rotary table stuff. It's not a very user friendly software, but with enough clicks it will do most anything the mind can imagine. We are, however, thinking about migrating over to Catia since they upgraded to an icon based system in V5, and Boeing uses it. We pay a good bit on translators in maintenance and man-power. There are some very nice CAM packages that work with Catia vs UG, but being really buisy makes it hard to take on the learning curve right now.

I used UG on a daily basis for many years. Learned on V9 and went up to V14. The learning curve is steep but the program could do anything. I programed LARGE 4-axis HMC's that ran parts that typically had cycle times in excess of 8 hours. I would love to be a UG user again. Those were the days that I used to really enjoy my work.

The major problem with UG programming is the amount of modeling needed to make it work right. Nothing sucks more than to select a surface, and see the surface area turn into 45deg's. I've found that creating a new through curve mesh, and splitting it in 2 pieces while losing parameters can sometimes fix the problem. It's nice to pay tons of cash to have to deal with this, but after 7 years using it I've figured out how to trick it into working.

edit: We're buisy enough right now that an extra programmer would really be nice. If you'd like to have fun and run UG again send a resume in. I'll see what I can do.

[email protected]

Dawson wrote:

If you'd like to have fun and run UG again send a resume in. I'll see what I can do.

Click to expand...

Thanks for the offer but I'm not wanting to relocate right now. But I'll keep it in mind 'cause my wife might like it because she grew up in Kansas.

I started using UG with NX and have moved up to NX4. Yes it has a steep learning curve, but it will make your coffee for you if you want. It has changed so much since the version you currently have. That is why I pay for maintenance.

Larry

We pay dearly for the maintenance, but aren't able to migrate past NX2 because of the customers we are receiving native files from. I really wish I could, and the Engineering manager is sick of hearing it.

I like how cavity mill was changed post V18 to know what a previous tool cut, and cut only where needed. It's made the roughing process quicker. Not only is it quicker for me, but also less wasted time on the mills.

I've been told that NX4 finally has a working Vericut style interface. I'm curious as to what else I'm not getting.

Dawson, I'm using NX3, and going to NX4 soon. You're right, it has lots of nice features, but boy am I having a time of getting my mind wrapped around this software! I come from a Surfcam/Mastercam background, and not much works the same.

I use Cavity Mill a lot as well. I've been using the in process workpiece (IPW) to help with reducing the steps that the first cutter leaves in the roughing process. I'm also starting to get a handle on planar milling and how the boundaries work, which is also handy. The thing that is so different, is that there are so many things to check, like retract heights, is the spindle turned on, etc. It's easy to forget things! I hope that get easier in time.

As for the verify in NX4, I don't know. My company insists on using Vericut to verify the G-code, and most of the guys don't even use the verify inside UG. I do, 'cause I like to get an idea of what the cutter's doing as I go.

I appreciate any further insights you and others have about UG.

I use Vericut directly from inside manufacturing in UG. It takes a Ufunc license and uses the .cls file to drive the cutter paths. I can run G-code through it, but it is slow to get setup.

For roughing I use cavity mill. Inside it I set a boundary, and also a trim boundary to keep the cutter from wanting to cut the outside of the die.

Here's a trick I learned a while back to get the cut levels to always fit. In your cut levels dialogue you'll see an odd number in the cut range box if you clicked on geometry. You can copy/paste this number in to the cut depth window and divide it by a number that approximates your desired depth per cut.

example:
1.035 depth but max of .050 per pass. Screen tip will tell you 21 passes, but it won't fit because it equals 1.050 and you'll be .015 heavy.

If you copy and paste 1.035/21 it will be .4929 per pass, and actually mill the final level.

For semi and finishing I only use fixed contour. It has boundary/planar functions aswell as surface area.

Thanks for the tips, Dawson. I'll take a look at fixed contour, as I wasn't sure exactly on which one of the contour choices was best. I think the other one is "area contour".

Here's another one:

When the guys in my dept. get a new job, they always look for a previous program that has similar operations and lots of cutters defined so they won't have to start from scratch. The old file is "saved as" the new part name, and all the geometry is deleted, resulting in a bunch of operations and a number of cutters. Then, the new geometry is linked into your new file from the engineering database (Iman, or Teamcenter Engineering I think it's called). The problem is, everyone's approach is different, and I may not like the choices the other programmers made. My idea was to make a .prt file with most of the cutters and operations we normally use, and call it a "seed file", and use that.

How do you and others approach this? Sorry to be so long winded!

I made template files for our most common machining tasks, and everyone pulls from them. This way tool #6 is always a 1.00 dia. ballnose. Also, all the machine control statements are in the operation for the tool. You only have to adjust the stickout and description of the cutter path.This makes it easier on the shop floor aswell since there is a good chance they will already have this tool set and ready to go from the last job.

To make your seed file into a templete you have to adjust it's template settings. The way mine work I can call up a MCS group and all the operations and tools come with it. It saves a ton of time.

For aluminum baseplates it will bring in the centerdrill,drill,reamer,tap,shellmill, etc. and I just need to pick the geometry and push generate. It takes less than 10 minutes from start to finish.