Best Approach For This Part In PowerMill

Hi,

Some may have seen my other thread where I'm finding my low level 3D CAM software wasn't cutting it when it came to having vertical walls (slots), as some would consider 2.5D features mixed with 3D contours. The fixed stepovers could not create accurate parts where I needed close tolerance (vertical walls) without creating such a small stepover it wasted a ton of time, where a smarter CAM package presumably could detect the walls and finish them at the right distance.

I reached out to some shops looking for unused software and have the possibility to buy an old PowerMill seat if I can confirm I can buy it resale... I've seen some packages, and this may be one of them, where you aren't allowed to sell the dongle. I don't see why it would be a problem and they didn't bring it up but I want to double check. It is a 2010 version that has been dormant since the guy that ran it left but I presumed it had more than enough features I need at this point. I did some online training and exercises via some PDFs I found and everything seemed pretty straight forward up until I got to put my hands on it with a sample part. When I went down to make sure it was running and try it before I committed to it and I could not solve my original issue:
Quickly creating a tool path for a 3D/2.5D hybrid part and have a finishing path that automatically finishes the walls and flats (horizontal planes) to the exact spec.

I played with the roughing (3D clearance) strategies a bit, and that seems plenty fine. But I spent most of the time trying all of the Finishing strategies and all the various options for them and could not seem to get an acceptable result. I'm sure this is due to my ignorance of the software because it seems quite robust.

Can someone give any tips on how to approach a part a like this? I have lot of these types of parts and shaving the cycle times down to last second is not important for me... but being able to open a part like this and have it ready for post in 15 minutes is.

The way I was trying to set it up in PM was a 7/16" Flat rougher roughing pass, 1/4" flat rest roughing pass, 1/4" ball finishing pass, 3/16" flat finishing pass (the slot on top is only .210" wide). Might not be the most ideal, but it was working well for me on my old software outside all the wasted moves due to the static stepovers. The other thing was I could not figure out how to do on PM is Rest finishing so the 3/16" would hit only the spots the 1/4" couldn't reach instead of redoing the whole part. On this part the only areas that are critical are the right angles/flats.

Is it standard procedure to use 3D Area Clearance as a finishing strategy to obtain the Rest strategies? The only reason I didn't consider doing that is the training suggested 3D Area Clearance is roughing only.

Thanks

I believe the Powermill license is not transferable. If you can transfer and want to update to current license it will cost you all past annual maintenance fees. This amount could possibly be more than the license purchase price starting fresh with the Delcam people.

Call your local reseller and talk it over with them.

There is a lot of options in the software bundles that can change the cost dramatically. Get What you need and start a relationship with your support team and I believe you will be happier.

Peace of mind is hard to put a price on.

Rest machining is roughing only.

you could create a stock model and a boundary based on the state of the model after any of your toolpaths to do rest machining. This is a very good functionality of powermill.

Check with Patrick from OneCNC west. He can show you how his software will do those parts. He's a very informative and extremely helpful guy (even after you buy his software!) 909 931 7811 No affiliation, just a really happy customer.

I think most CAM users cross this bridge at some point or another... Do I use 2D tool paths or 3D tool paths to cut my 3D Model. As we all come to know, some features can only be cut with 3D tool paths and others could be cut with 2D or 3D tool paths. So it comes down to process, lead time, and opinion.

As an example, you may be able to produce a shorter run time using 2D tool paths, but it may result in 3X the programming time ( sitting at the computers and setting up your tool paths ). Vice Versa laying down 3D tool path can be very quick to setup but can result in 3X the run time. ( the time it take to run the part on the machine) If you are making 1 or 2 parts then it will be faster to spend 15min setup time and 1 or 2 hours or run time, then it is to spend 1-2 hours of setup time and 30 mins of run time.

Using all 3D tool paths on a 3D model like yours will result in a finished par, but you could experience some out points.

Problems that can occur:

3D Tool Paths do not use G41/G42 so if you have critical tolerances in specific areas, you lack control to dial them in.
Run Time can be longer using "catch all" tool paths

Some Advantages:

Quick to setup
Easy to make changes

2D Tool Paths do provide more control, but require more effort and thought. Gouge Checking is not common for 2D tool paths. So you need to pay attention to your lead in and outs. You may also need to manually layout "parts" of your paths to get the results you are looking for. If you need to make changes it's not as automated as selecting a model and computing.


In some cases you will use 3D tool paths to machine most of the part, and 2D tool paths where you need clean up areas. Slots and other vertical walls are easy to clean up using a profile feature. You may find yourself combining 2D and 3D tool paths to get the part off your bench.

I think when it comes to CAD CAM support is important. So IMHO it would be better to purchase a package with the support than not. You may get a great deal on some older software, but having a team to answer questions can be better for you as a newer user to CAD CAM ...

As far as CNC West goes, I would agree Patrick is a great guy and can help you Pre, and Post sales. As long as you are in his territory you are good to go!

If you want to upload your file via drop box etc, I am sure more than a few of us could lay down some paths and make some recommendations.

Delcam products require a PAF file, (product authorization file) I do believe it expires after an "x" amount of time, for us I believe its a year. Then things will probably get ugly and stop working.

Thanks for all the replies. I actually started getting more comfortable with the software and as such became more impressed with its features. Indeed, stock models is a great feature!

Figuring out the licensing details was one hurdle, but I was only going to worry about it if I decided to pursue it. Although it is pretty capable software compared to what I was using, after demo'ing a couple new packages it was night and day in toolpath efficiency. Since I am only working with 7.5 HP I kind of need all the efficiency I can get. PM wanted to plunge into the piece and full width slot (or trichodial if overload selected), where the smarter offering would attack the open pockets from the outside with adaptive cutting. The downside is to get the highest efficiency in the HSM toolpaths I would need a newer control, and I'm running a 25 year old Fanuc 0M that gets dicey past 30 IPM even with liberal arc fitting tolerances in the tool paths.

Making the leap from mostly manuals with some playing on toy sizes CNCs to a real VMC has been more than I bargained for in terms of what I've needed to learn in the process. Of everything I tried that would fall into the more "old school" style CAM packages, where you have lots of control and options over every aspect of the tool path creation, but not neccessarily as many "smart" features, at least not in the 2010 version, I would say it is the best I tried by far. If I hadn't discovered HSMWorks I would still be interested in it. Instead of building on this thread I am going to create a new one since PM is now off my short list but I have a couple questions pertaining to a pair of different offerings before I pull the trigger on one of them.

thebee said:

PM wanted to plunge into the piece and full width slot (or trichodial if overload selected), where the smarter offering would attack the open pockets from the outside with adaptive cutting. The downside is to get the highest efficiency in the HSM toolpaths I would need a newer control, and I'm running a 25 year old Fanuc 0M that gets dicey past 30 IPM even with liberal arc fitting tolerances in the tool paths.

.

Click to expand...

I can't believe that PM wouldn't let you come from the outside in. I'd be very surprised if it didn't.

Matt_W said:

I can't believe that PM wouldn't let you come from the outside in. I'd be very surprised if it didn't.

Click to expand...

Of course it will. There really isn't a lot that PM _won't_ do. The million dollar question is _how_ to ask it. I try to learn something new every week with PM. It hasn't left me wanting yet.

In Powermill it's called Vortex strategy, in the roughing area, it will indeed do what you wish, and very efficient. And make sure you have the approach outside box ticked.

5 axis Fidia guy said:

In Powermill it's called Vortex strategy, in the roughing area, it will indeed do what you wish, and very efficient. And make sure you have the approach outside box ticked.

Click to expand...

Vortex didn't exist in the version he's using. ( PM2010 ) Still, he can use just about any of the roughing routines, while noting your point - to enable PM to approach from outside.