I was wondering if I can get some unbiased feedback on how Gibbs performs with 3d work like mould making and fixture building....cnc wise.

I am looking into a multitude of cam systems and need some advise from real users, not just salesmen.

Thanks.

Hi Krusty Krab,
I cannot give an unbiased reply about GibbsCAM as I have been using GibbsCAM products since 1988. I can tell you that I build a lot of permanent molds with core boxes, core boxes with cope and drag sections. Some of the molds have a part B/P available, some do not. I digitize where I can. I build the finished casting or finished core in Gibbs and can control the shrinkage ratio according to the material cast. Gibbs has a parting line tool that is a great help. Creating a 3D tool path is easy in Gibbs. I use Fadals and they handle the mass of code with no problem. I cannot compare Gibbs to any other systems as I quit looking in 1988.

Hey Krusty -

All I make are molds, patterns, masters & associated fixtures for the composites and thermoforming industry. 3D tool paths are very easy to create in Gibbs. Also, Gibbs has a big version update, V8.0, in the works that will focus on 3D milling and high speed machining.

I had someone over for a demo yesterday and I really liked it. He didn't really push it as a powerful 3d cam ware, but he didn't knock it either.

There was one thing that turned me right off of it however. The toolpaths that are created want to go up to safe z between each and every step over. Is this so, or was I just not shown properly?

Obviously this would present a huge waste of time.

Here you go, the truth the whole truth and nothing but the truth....


GibbsCAM is a GREAT all around product, it does 2D VERY well and is very flexable. You can make it do just about anything anyway you want. This is importaint because every mold/tool and Die shop I have sold GibbsCAM to have a large amount of 2D work as well.

As for the 3D toolpath. Here are the good and bads:

Good

Very SIMPLE
Fast toolpath calculation
respectful use of associative toolpath
Good Roughing Paths (not a ton of retracts)
Flexable
Can be proficent at it in less than a week
Many more.....

The BAD

Not suited for LARGE Mold work, IP's, Dash Panels, Facia Molds
This is because there are not many "Optimizing" toolpaths. The ones that find and 3D re-Machine the extra material.

Lack of Shallow/Slope Miling
Looping Toolpaths (Lace Cutting)
Skimming Retracts


In all, If you are doing VERY Large, VERY COMPLEX Molds/Dies you should look at a specialized product. The 2 best in the industry are WorkNC and PowerMill. (I have used them both)

If your work fall into slightly smaller work and you need to use Solids for modeling and cutting then GibbsCAM is a Great fit for you.

As some one said before, Gibbs is adding numerous 3D Milling upgrades and additions to the product. (Slated for V8). The stuff that they are talking about will make most if not all the above information useless. GibbsCAM should be close to a one stop shop for all your milling needs.

Your comment about the retracts, I think the operator did something wrong, Most of the Finishing cuts in GibbsCAM stay down very well and retract only if needed. The roughing and Z Level finishing have some retracts but no more than other products do.

Good Luck

GG

Hi Krusty Krab,
The Safe Z retractions are part of a few options to choose while creating a tool path. "No Retraction" is also available.

This can somtimes be a bad thing. The toolpath can violate the part if this option is not turned one.

You need to know the right part deffinition to make this work without error.

GG

Where you do have Z retracts you have the option to either let the tool FEED back to the part or RAPID to the part at a distance that you set. This can be a big time saver.

Sorry guys, but any program that doesn't provide skim moves on retract is a severe time waster.
Especially when you are finishing fixtures to zero stock with smooth finishes.
You can imagine the tens of thousands of retracts involved. This could waste as much as 5 hours or more per job.
I think I will keep looking.
Thanks for yer advice.

I don't think you understood my comments.

It shouldn't matter when "finishing fixtures to 0 stock with smooth finishes", when finish milling, there should be little on no retracts involved anyway. The only ones would be to re-position to another area.

If retracts would add 5 hours or more to the job, then you need to look into changing the programming or get a faster machine.

Look at the software again, the retract issues should NOT be issues for your finishing.

GG

gibbsgod,

If you are programming a linear toolpath on a large sweeping 3d surface with a 1inch ball cutter, the stepover required would be about .3mm to achieve a smooth finish.
If the toolpath is retracting up to safe z between each stepover then that IS a waste of time.
Of course, if you choose to machine using zig-zag, then it wouldn't need to retract. Unfortunately, zig-zag machining doesn't result in a nice looking finish when it comes to metals, it will leave directional change lines.

I will get another look at the software, when the demo disk comes, however, the rep that showed me the software said that the toolpaths retract to safe z between stepovers. Perhaps he's misinformed?

No, you were not misinformed by who ever showed you the software. In a oneway cut (Box Cycle, climb only etc...) the tool will rapid to the specified Z plane to return for the next stroke.

I have not yest seen a software though, that will skim these kinds of moves. (But I have never looked for thie either) In most cases, the "SKIM" moves are reposition moves to another location on the part for more cutting.

I would like to see a one way cycle with skim moves included. I wonder how much time to would really save, is a straight linier move faster than a move that is following the contour of the part on every cut?


Good Luck

GG

Skim moves are available in Mastercam, CamWorks, Machinist, Powermill, Worknc. There are others that I haven't checked into yet.

As far as linear versus contour mode of machining surfaces. I don't think the actual toolpaths will vary much in the amount of time each take. It's the rapiding up and down that I am concerned mostly about.

I already know how to optimize my toolpaths with respect to tooling, material, shape, and locality.
I have been doing this for almost 13 years now(I think), and I can tell you that if your toolpaths contain some 10,000 retracts to cut an entire job, at about 2 second per retract(probably more) you've wasted 5 hours!!!!
By the way, it would be cheaper to spend another 4-5 thousand dollars on better cam software than it would be to replace both of my machines. (They only have about 350-400ipm max feedrate)

Krustykrab,
Does Mastercam (better cam software) cost 4-5 thousand dollars more than Gibbs?

I made no indication that Mastercam was better than Gibbs.
All I said was that it has skim moves on retract. I personally don't like Mastercam, the interface bothers me and the inability to change the view whilst displaying the toolpath is a definite no-no.

But, yes Mastercam does cost about 4 thousand more than Gibbs, once you add on the Solids add-ins and their respective maintenance charges.

PLEASE DON'T BE MISTAKEN HERE: I am not here to knock any Cam software, I am on a quest for the RIGHT SOFTWARE FOR MY SHOP. Strong points will be functionality, functionality, and functionality.

Input regarding pro's and con's of cam wares is appreciated, defensive cynicism is not.

Originally posted by krustykrab
I made no indication that Mastercam was better than Gibbs.
All I said was that it has skim moves on retract. I personally don't like Mastercam, the interface bothers me and the inability to change the view whilst displaying the toolpath is a definite no-no.

But, yes Mastercam does cost about 4 thousand more than Gibbs, once you add on the Solids add-ins and their respective maintenance charges.


krusty,

Here is my opinion on this matter. I've tried to stay out of it, but there's been some things said here in the Virtual Gibbs Forums which are mis-leading and/or false so I will step in and clear them up a bit. ;)

I've used both for many many years. (Do a search, you'll see some of my reasoning behind this educated and multi-faceted opinion :cool:

Mastercam will release "X" likely this year, with what some would say is a complete re-write, including the infamous GUI. Personally, I can flow thru the (old) Mastercam GUI as fast as I could with Gibbs. (Trade-offs on both sides, obviously..)

Also, I'm not sure if you're talking about changing (rotating etc) views while backplotting or verifying, but you CAN do it in BOTH.

Also, Gibbs, from what I've seen, has still failed to produce an intuitive, complete and useful free post editing procedure, and is still highly limited in it's ability to create toolpaths 'just the way I like them'. (We'll see in the next big release). The toolpathing in Mastercam is, IMNSHO, better and more accurate than Gibbs. Trade-off for time? Not any more if you're on maint or move to X. ;)

Gibbs is a great product, don't get me wrong, but Mastercam is better for nearly everything I've used either product for in my somewhat limited career. BTW, I've used Gibbs in over 60% of my 15ish year career as a programmer, and we used the old Mac GibbsNC/CAD/CAM for the 5 years I spent as a setup guy before I moved into programming.. That system r0x0red meh b0x0rs, but that's a different story. :)

'Rekd

Originally posted by Gibbsgod

I have not yest seen a software though, that will skim these kinds of moves. (But I have never looked for thie either) In most cases, the "SKIM" moves are reposition moves to another location on the part for more cutting.

I would like to see a one way cycle with skim moves included. I wonder how much time to would really save, is a straight linier move faster than a move that is following the contour of the part on every cut?


Good Luck

GG

GG, you can set retracts to either incremental or disable them completely, and have the tool 'follow' the surface to re-position itself between cuts ;)

'Rekd

Thanks Matt for your comments.

I am aware that Mastercam has more features than Gibbs, and, does everything we need to do.
As far as rotating the view while backplotting, could you let me in on how to do that. I just couldn't figure out how to do that without closing the Operations Manager.

The ops manager closes when you enter backplot.

What I think you're looking for is a modeless ops manager. Meaning you can access other functions of MC while the ops manager is open. This won't be available until X, and has also been one of my pet peaves about Mastercam but is a small price to pay, and there's light at the end of the tunnel. ;)

'Rekd

Ok OK, I can amend the comment about the retracts. I'll go along with Rekd on this one.

I think the Post Haste opton for FREE posting is good + at best. You need to realize that this is in the software to addess the user editing post issue. (Kind of like a check box) I have used them, wrote them and edited them for Mills and lathes. They are very straight forward and fit the needs for MOST (I said MOST) users that just want to change a few things.

I still feel that the GibbsCAM posts (that you buy) are better. These are well suited for the users that can't write their own name, don't have any programming experiance or FLAT OUT "DON'T KNOW WHAT THE MACHINE NEEDS" to run.

With the avalible opions (upgrade to a FULL Function version) from PH in the 7.3 version I think this issue will be resolved much better.

Also, if you are a larger install, you could always barter for the Compost compiler. Then you would not have ANY ISSUES!! you could do anything you want.


As for MC vs. GC...... Well this has been going on for EVER and will continue for a long time. I think of it like this:

In most cases (for general machining) any customer could buy either and get the job done. I think people still decide on overall use, product layout, how easy it looks to do things (this is a loaded question, most resellers can make anything look easy in any software), COST, support, options (most try to compare packages option to option, this is a mistake. This would take forever and would still be a draw (with all the give and take)) and general feeling.

I guess what I am trying to say is that you can't go wrong with either product, just make sure that the MAIN type of work you do taylors to the strong points of the product you select.

Another option, Gibbs has a 60 day unconditional return on their sotware. Make MasterCAM match it, then give them a try. If your first choice is GibbsCAM use it for 59 days , DON'T LIKE IT!! Return it and give MasterCAM a shot. (or vice versa) If neither work SHOP MORE!!

Good Luck.

GG

Another option, Gibbs has a 60 day unconditional return on their sotware. Make MasterCAM match it, then give them a try. If your first choice is GibbsCAM use it for 59 days , DON'T LIKE IT!! Return it and give MasterCAM a shot. (or vice versa) If neither work SHOP MORE!!

I wasn't aware of that. Very good idea, and somewhat un-heard of in this industry. Kudos again to GC!

Yes, the MC GC debate will go on for a long time. Both are great products, but if you look at CIMdata, you'll see that Mastercam has 70,000 installed seats world wide, which again makes it the most popular by more than double the amount of installed seats of it's closest competitor. Also note that Gibbscam is not on the list, and falls somewhere short of 20,000 seats.

http://www.mastercam.com/camzone/newszone/Cimdata/Industpie.jpg

BTW GG, I don't know how long you've been use Gibbs, but have you used the old mac version I mentioned before? I'd like to see them add some of that toolpathing functionality back in the newer versions.

'Rekd

First the OLD Version.

YES I DID (The Gibbs SYSTEM). I also wish they had more of the original features in the latest versions. I think the Parasolid move was a great one, but to leave out the best of the GS was a slight mistake.

I am awaiting the addition of some of those options. I have used it/sold it and done testing (for Gibbs) on Gibbs for 9 years now.

As for the mastercam seat count. This has always seemed very weird to me. I heard people talking about how to count seats installed.

The best I know that would make things seem real (but MasterCAM would still have a much higher seat count) is this;

When I sell a Gibbs seat of mill, that counts as one seat. When that same user adds lathe to the mill seat. This is still one seat to Gibbs. (one exacutable one seat!!) If that same user several years down the line adds Wire to the mill/lathe seat. Still ONE SEAT. (one exacutable, one key all licesed to the same computer).

Now for MC. Same senario except each option added is a seperate exacutable, hence another seat. If you do that math, things come into clearer view. MC still is GREAT at giving away educational seats (these also count) which has been the BEST Thing they could have ever done. Their name is EVERYWHERE!!


Ever wonder why MC seat count is so big compaired to others like UG, PRO/E CATIA?? These companies have seat counts in all MAJOR accounts, Boing, Ford, GM Chrysler and others. All these installs have HUGE seat counts and the number put them about 1/2 of mastercams isntall.

Just doesn't seem right to me. The senario I was talking about as far as seat count would make sense.

Thats my input right or wrong, I don't think I could ever get a lagitament answer on how things are counted. It does seem fesable to me though.

GG

Interesting points, and it somewhat validates my own questions concerning the same thing. I'll dig into it a bit and see what I come up with.

'Rekd

Having built injection molds for many years, I cannot recommend Gibbscam for 3-d machining. It does a poor job with vertical and near-vertical walls with the Z-axis frequently hunting up and down. I have had disastrous results doing lace-cuts in multi-cavity molds when using either patterns or the "translate toolpath" plugin- after completing the original path, it gallops off in the wrong location and busily mills miles away from where it should be even though the render screen indicates all looks fine. Also, the "shrinkage" calculation is way off. I have found this to be true on every computer and every version of Gibbs I've used in the last 3 years. (Draw a 20 inch circle, do a 1-1/2% shrink and then measure it. It should be 20.300, not 20.3046) The annoying aspect of all this is that Gibbs denies that there's a problem. The only other CAM program I've used is Surfcam, and for moldmaking it has it all over Gibbs. On the other hand, for 2-d work, Gibbs is great-picking geometry is a breeze.
That's my 2¢ worth.