What's new
What's new

WorkNC vs. Powermill (3ax), which and why?

Harri

Cast Iron
Joined
Jun 1, 2006
Location
Finland
Looking for a powerful 3 axis CAM solution for general prototyping and high precision optical surfaces. Both candidates look nice and powerful, both have good local sales & support. One month demos are available, but that's only good for a honeymoon. If anyone has a lot of experience with either, I'd really appreciate some input on both the good and the bad. It's a big investment and I'd like to get it right ;)

Top priorities:

-great code
-ease and automation of code creation (prototypes; need to get the job done quickly without fighting bugs and workarounds)
-speed (64 bit and multicore support)
-good with high-tolerance freeform surfaces
-good post processor editor
-good support

Many thanks/Harri
 
Hi Harri, can't help you with the Powermill software as I've no personal experience of it other than to say a company I worked at had it and it worked well for them.

To answer your specific questions with regard to Work NC:

Great Code: I've used WNC for over tens years and have cut thousands of parts with it including some very complex parts and can honestly say hand on heart I've never ever had any bad code. Any issues have been either machine or operator based problems, not software.

Ease of automation of code creation: WNC allows you to set up machining templates that you can easily adapt to whatever you're machining. Like most mould toolmakers I machine a wide variety of materials with soft materials like copper/graphite through to fully hardened tool steels, once you've built up your libraries you can use them over & over again.

Speed (64 bit multicore support): See previous post:typing:

Good with high tolerance surfaces: WNC is excellent for this sort of work, over the years we have made plenty of parts that have had to have not only optical surfaces i.e. see through polished surfaces but also with specific optical properties like focal points, mapped surfaces, lightguides, LED diffuser/lenses and have all been good. Perhaps the best feedback is from mould polishers (who get to see a wide variety of tool work) making favourable comments on the quality of our machined surface finishes.

Good post processor editor: Another good point, over the years we have tweaked and modified our posts ourselves, all with technical guidance from WNC support. You can open the post file in a text editor like notepad and edit yourself, so should not be a problem.

Good support: Very good here, but that's not to say it is where you are, it all comes down to the people you have to talk to and their attitude.

Hope this helps.
regards John
 
Thank you John!

That really helps, exactly what I'm looking for.
edit: before I get completely carried away, what do you like least about WNC? Annoyances?

Harri
 
Last edited:
What I least like about WNC is more to do with modern machining in general. I don't like sitting in front of a PC for hours on end so I tend to look at CAD/CAM as a necesary evil. I get far more satisfaction from being in the workshop making stuff. I'm old enough though to know that things are a lot better than the old days, in a previous life I used to use a big Cincinnati Hydrotel as well as various pantographs and I don't miss them a bit.

To answer your question about WNC one annoyance I find is that if you chose to machine an area by selecting the surfaces the cutter doesn't always go right to the very edge of the surface, I'd like it to use the edges as a boundary curve and have options of being able to get the cutter to overlap these boundaries by a set amount. It's not a big problem because you can make the cutter do exactly this by using and selecting bounding curves, just a niggle.

One other issue is specific to electrode creation, when you right click an electrode you can select to return to its parent geometry, it closes the electrode and its UCS and takes you back to its parent geometry and its UCS, sometimes it can get a bit lost doing this, nothing serious but a niggle none the less.

Thats all I can think of for now.
Regards
John
 
Last edited:
I am a powermill guru, it is wonderful on the things you list, including one of the most fantastic gouge free and collision checking-avoidance when it comes to cam packages. Work NC is also very good software from what I understand, I have no experience with it. I could ramble on for hours on the PM system, I would suggest going with who has the best support and maintence cost in your area. Both systems will have some quirks, both good and bad. If you have any particular questions, feel free to ask, remember sales guys are just that, they live in demo land..
 
5 axis Fidia,

I'd like to ask the same question I asked John: what don't you like, what would you change if you could?

Thanks/Harri
 
Harri, My first gripe would be the 2d toolpaths, Delcam makes the easy things hard and the hard things easy so it would seem, the 2d is not difficult by any means, just a little cumbersome to get the hang of. I do all 3x and 5x work, so I personally could care less, if you used it everyday you might get the feel for it, I do it like once every few months so I fumble around a bit. Another annoyance would be the viewmill, in my opinion its slow and dated, although they are working on it.. Some strong points would be the lack of gouges, never, and I mean never does it gouge anything your not anticipating, same for collision checking, its bulletproof, I collosion check some toolpaths with the holders only clearing by .015 in some instances. Another strong point, all the new versions they come out with, 2 full versions a year and about 4 or 6 service packs along the way, in other words, if there is something you don't like, it wont take long and it will get updated. One last strong point, all the different finishing and roughing strategies.. I count 29 different finishing strategies alone, not to mention custom toolpaths you can make with patterns. If I ramble on anymore you might think I sell the stuff.. any other help just shout.
 
Thanks Fidia!

I'll probably have some questions in a few days..

Today we had our WorkNC demo and it left some unanswered questions:
There seems to be no way of automatically calculating speeds and feeds for a known material, just a box for SMM and RPM, surely the sales guy has overlooked something?
He also claims no subroutine support and no work coordinate support for posting into different systems (G54, G56 etc.) I'm hoping this can't be true.

Also speed/feed optimization seems to be missing, unless it's part of the optional NCSpeed module. Another deal breaker is lack of G8x support without buying a separate module. I mean really, extra $$ to use G84?

And a final question: simulation looks really chunky and Rest material visualization seemed to offer two options: a less than useful mesh draped over the part or a low-res approximation of what's left. Again, I think I must be missing something here... Unfortunately the demo seat we have is the older 32 bit version, lacking the goodies you guys are raving about in the other thread..

Harri
 
Hi Harri
The cutter library allows you to enter a surface speed for a known material and the feed per tooth for the type of operation your want to perform. The cutter library is key to automating your cutter paths later on. Obviously everone has their prefered suppliers for the types of cutters they use, it allows you to enter all this info incl order/part numbers. The key to building a cutter library is that you can edit a particular cutter for one material change the parameters to suit another material and simply save it in another library for the new application. Library supports all types of cutters like tapered, reinforced, undercut lolipop and will collision check 100% reliably the cutter against gouges as well as the holder.

Bit stumped on sub routines, do you need them in a CAM package? To me they are something you do on a machine control to save entering lots of data, where's a CAM package will just crunch the numbers. Can you explain more? G54 shifts are not something I do as practicly everything I make is one off. If you want multiple parts you could, as a work around, either model the multiple parts and machine them, or cut & paste your code in a text editor with the shifts in there. Work NC do have a module called multi part machining that does just that, something you can look that up if that's what you need?

Speed and feed optimization is, in my opinion something you refine in your library with experience of the type of work you do, it's always a balancing act between cutter life, work quality and machining time. Get it right and you will never ever break a cutter. To improve matters if your machine supports them you can post G05.1 surface finish G05.2 data smoothing.

I have a late Hurco that's so easy to drill & tap one off parts that, for me, I can't see any advantage in CAM programming them. I can switch from nc code to conversational with the same set up on the VMC. I do know for a fact WNC has a drilling manager with feature recognition that should do what you want but I've no experience of it.

Believe it or not but I hardly ever use the simulation or rest material viewers, and I agree they do look clunky. If I have any part to make the best way to approach it, in my opinion, is to quickly but thoroughly inspect it with the analysis functions, this will tell you everything you need to know about the part, you can then select a previous machining sequence to use, or tweak a little, to get the job done. When you rough out the stock model will get the next smaller cutter to remove just the areas left, move onto the flat surfaces and finish them, finish machine, maybe optimise some paths and finally rest material machine what's left, job done, all in a saved sequence specific to the material being cut. Any issues with cutter lengths the tool holder collision will tell you straight away so you will know safe cutter lengths. Check it with the simulation if you really want to.

A few questions for you.
What sort of prototype work do you do and what quantities?
What machine will you be using?

The reason I ask is we have a SWI dual purpose mill that is both 2 & 3 axis and for prototype work it takes some beating.
Like 5 axis Fidia guy said, CAM packages make hard things easy but can make easy things hard

John
 
Harri, do you have a Gibbscam reseller nearby? All the features that you listed that Work NC was not able to show you in the demo, Gibbs does do. We use it on simple 2 axis one part jobs all the way to 5 axis production runs.
 
Munruh,

Gibbscam wasn't on my list and you're welcome to correct me if I'm wrong, but I didn't realize it's in the same class. Choosing CAM is a tough job at best of times and I've managed to narrow the list down to two candidates, based on reading posts here, testing and intuition. (After looking at Tebis, Mastercam, HSMWorks, Esprit, NX and a few others).

I'm using OneCNC now, and for the price it does a great job. However, you get what you pay for, and I'm looking for the best possible solution, particularly for high tolerance 3D work. I don't want another heated OneCNC argument and I'm not bashing anything, just looking for more speed, control and power ;)

I also imagine most of the things left unanswered by the WNC demo do have a solution, waiting for some users to chime in..

Harri
 
John,

Thanks for the time and info. We have a small Mori Seiki VMC and a specially built machine for lenses and other small stuff. We'll do almost anything in our size range so it's difficult to be more precise. Mostly small parts in aluminium, stainless and various plastics. Batch sizes usually 1-20, sometimes a few hundred.

The SWI sounds interesting, got a link or a pic?

Harri
 
Harri

Heres's a pic from the internet similar to our DPM (Dual Purpose Mill). Like I said for prototype work hard to beat. Things like optical surfaces and intiricate electrodes, definetly not, general shop work, prototypes...perfect.

John
 

Attachments

  • Duel Purpose Mill.jpg
    Duel Purpose Mill.jpg
    73.4 KB · Views: 1,342
Munruh,

Gibbscam wasn't on my list and you're welcome to correct me if I'm wrong, but I didn't realize it's in the same class. Choosing CAM is a tough job at best of times and I've managed to narrow the list down to two candidates, based on reading posts here, testing and intuition. (After looking at Tebis, Mastercam, HSMWorks, Esprit, NX and a few others).

I'm using OneCNC now, and for the price it does a great job. However, you get what you pay for, and I'm looking for the best possible solution, particularly for high tolerance 3D work. I don't want another heated OneCNC argument and I'm not bashing anything, just looking for more speed, control and power ;)

I also imagine most of the things left unanswered by the WNC demo do have a solution, waiting for some users to chime in..

Harri

Harri, Gibbscam is in the same class as Mastercam and Esprit if you are looking in that price range.
 
Some previous posts of mine on PM -

Zahnrad Kopf said:
There's a *LOT* of things I think PowerMill just does better than anybody else's software, but yeah... the toolpath editing is just F'ing incredible. First time it was shown to me my jaw just went slack while I drooled on myself. It is VERY powerful stuff. My time spent programming was literally cut in half during my first steps with it, in comparison to MasterCAM. It only got better from there. Nuff sed. Suffice to say I am very biased.

Zahnrad Kopf said:
People usually point out that people rave about what they use, mostly because it's what they are used to, and often because it's what they have to use, while also being mot comfortable with it due to both. With that said, I have the option to use a few different CAMs if I want, and can't find a reason *not* to use Declam Powermill. I honestly love it.

Now, here's the bad -

If you want to be efficient with it, and have any hope of enjoying working with it, you'll have to take all your preconceptions about *HOW* your CAM works and toss them, right from get-go. This means everything from nomenclatures of things or features to little things like "undo"ing things or having "windows"-like widgets. (like CTRL+Z)

The really good -

If you can get past that, you'll have some very, very powerful control over toolpath and strategies, and even portions of them. Great stuff. There's not a lot you can't do with it.

Zahnrad Kopf said:
Most oft, I'd be in agreement with you. In that vein, I'd recommend a demo of PowerMILL to see what you'd think of it. I've found that it's pretty adept at these sorts of things, too. Even if one of the standard strategies *would* go into places you might not desire, just to get those types of moves, you can simply choose that section you do *not* desire, and tell it to remove it as toolpath.

And it does. Very nicely, too.

Don't like how it feeds into a corner? Choose that section of toolpath and change the feedrate. ... or its direction... ... or its entry... ... or its exit... ... or all of the above... This was one of the very first things that I was exposed to with PowerMILL.

Zahnrad Kopf said:
A little late to the game, but I have to throw my vote for Delcam's PowerMill, too. UG and Esprit are the obvious big name packages, as well. As others have already said, PowerMill can seem very daunting at first, but my opinion is that it's mostly because they do things the right way. NOT the way people are USED to. And they don't fsck around with trying to make the interface windows-like. If you can "turn off" what you "know", and have an open mind as if you were learning for the very first time, without the prejudices of what you have come to expect, you will quickly acclimate to it, and wonder where it's been all your life. In my opinion, it is VERY underrated for how powerful and configurable it is. Just my personal opinion.

Fidiaguy's observations are spot on, as well. 2D stuff could use some work, but it's rarely an issue. Viewmill is a slightly clunky, too. To be honest though, these are such small pieces of the larger picture that they're not of much concern in my book.

I've also been taking advantage of PowerMILL's tool library and macro/scripting features a lot, the last 12 months. There's a lot one can automate and make one's life so much simpler with PM. Really makes programming a short task that RARELY results in something that needs a second look.

It really comes down to simply choosing HOW you want the tool to engage the work. PowerMILL takes care of all the little things we used to have to concern ourselves with. :cheers:
 
Last edited:
Almost forgot - the post processor editing was a bit foreign to me at first, but I've gotten used to it and write/modify posts fairly well these days. It's not too hard to learn. Hope that helps.
 
Camtool anyone? I don't know about the other softwares mentioned but it uses true surfaces as opposed to a 3d wire mesh. More accurate. We machine molds and get the best finishes from this software, its main focus is hardmilling for molds and dies. Its not as popular over here I don't think (Japanese software) but definately worth considering.

It has full libraries for hitachi, osg, union, mitsubishi, and a few other top cutting tool suppliers. Part numbers directly from there catalogues. Also calculates feeds and speeds based on material hardness and type of endmill being used, bull, ball etc.

CAM-TOOL - NC CAD CAM Software - Canada
 
Narbo,

Interesting product, horrible retro-website ;)
What sort of price range are we talking and what's support like?

Harri
 








 
Back
Top