[Dan B]

With all the positive feedback about OneCNC, I can't help but wonder how it compares to WorkNC (which we have been using for 12 years). I came up with a list of, what I feel are necessities in CAM software. How does OneCNC measure up (if a 30 day demo was possible I wouldn't be asking this here )

Here it goes:

1) Does OneCNC have a tool library that contains a variety of parameters for that tool (speeds feeds, step-overs and step-downs etc)?

2) Does OneCNC have the ability to edit toolpaths with windows or closed curves? In other words, can I window on a toolpath and delete what is in the window?

3) Can you work while the path is crunching or do you have to wait?

4) Can you isolate areas and re-order without re-processing?

5) Does OneCNC have automatic rest model machining (actually I'm pretty sure it doesn't, but I'll ask anyway)

6) Does OneCNC have user-friendly post-processor?

7) Does OneCNC have the ability to easily create a view normal to a surface for multi-axis positional toolpaths?

8) Does OneCNC have a 3d stock model (updates from any angled cut)?

9) Does OneCNC have the ability to save toolpaths and load them when appropriate (sequences)?

10) Does OneCNC have climb and conventional options for all toolpaths?

11) Does OneCNC have mirroring capability (preferably after editing so as to preserve edits)?

12) Does OneCNC have editing without having to re-calculate your entire path (sort of related to question 2 and 4)

13) Is OneCNC able to generate some sort of documentation for the machine operators?

14) Does OneCNC have a holder library and do reliable collision checking?

15) Can OneCNC do batch processing (for example, run paths at night)?

16) Does OneCNC have the ability to engrave with step-downs?

17) Does OneCNC have decent machine simulation with user configurable machines?

18)Does OneCNC have a "Cursor guide" that has an adjustable radius definition used as a guide for creating boundries etc. ?

I know it's a long list, and I appreciate anyone taking time to address some or all of these points.

Thanks,

Dan

[HuFlungDung]

1) Does OneCNC have a tool library that contains a variety of parameters for that tool (speeds feeds, step-overs and step-downs etc)?

***Yes***

2) Does OneCNC have the ability to edit toolpaths with windows or closed curves? In other words, can I window on a toolpath and delete what is in the window?

***This sounds like a question arising from a particular technique which you are used to in other software, which makes it difficult to answer. Part of the standard fare is wireframe toolpaths, which you create. Every modification requires the process to be created again, but this is quite painless, as it takes a half dozen mouse clicks to complete. The other toolpaths, using Solid Machining Technology are what I call "surface aware" and are totally automated, but still you can change the approach type, cutting depths, stepover, tool, work offset, rpm, feedrate or if you choose to work in automatic extents, you can change the size of those. You can also use a hand drawn boundary and work inside, on, or outside that. A boundary modification requires that the process be regenerated, again a half dozen mouse clicks. Complex boundaries are not typically necessary, ie., many users go to a lot of needless pain about this, and spend more time having the tool make entry points than it would just going round and round ***

3) Can you work while the path is crunching or do you have to wait?

***Yes, you wait***

4) Can you isolate areas and re-order without re-processing?

*** In SMT processes, all except Z level, you can select a single surface of the model, and the toolpath will generate for just that surface, with interference checking going on around its edges. You can drag and drop processes in the NC manager to change the order of operations***

5) Does OneCNC have automatic rest model machining (actually I'm pretty sure it doesn't, but I'll ask anyway)

***It will search for the rest areas, and you set up processes that will perform SMT operation on that area. I suspect that the nature of rest machining requires human decision to determine the appropriate direction which would be best anyways, since the rest machining processes are like a slope delimited planar toolpath: you sketch a boundary around the area, and then tell it between what slope elevations to machine between. You can set direction and stepover to suit. I don't really see how this could effectively be automated, as there is too much critical user parameter input required to get the proper results. That is just IMO ***

6) Does OneCNC have user-friendly post-processor?

***Definitely***

7) Does OneCNC have the ability to easily create a view normal to a surface for multi-axis positional toolpaths?

***Yes, XR2 now uses a what we call a construction plane. This can be set quickly on any desired surface, and then select 'Plane view'.***

8) Does OneCNC have a 3d stock model (updates from any angled cut)?

***Not at this time. The automatic extents are the stock size, and they define a simple 3d rectangular cube.***

9) Does OneCNC have the ability to save toolpaths and load them when appropriate (sequences)?

***The NC manager saves all processes in tree view. They can be dragged and dropped into any order. You can also merge files containing machining processes where appropriate. The processes will be imported. I think this is one of the key reasons that boundaries and 2d geometry are 'locked' with the processes, once they are created. This makes them portable.***

10) Does OneCNC have climb and conventional options for all toolpaths?

***Yes***

11) Does OneCNC have mirroring capability (preferably after editing so as to preserve edits)?

***You can mirror any geometry or model. New processes must be created for the new geometry or model.***

12) Does OneCNC have editing without having to re-calculate your entire path (sort of related to question 2 and 4)

***It always recalculates the toolpath at the end of the edit wizard. This is carried out on a "per process" basis, not the entire machining program. ***

13) Is OneCNC able to generate some sort of documentation for the machine operators?

***Yes, a job sheet is printable***

14) Does OneCNC have a holder library and do reliable collision checking?

***Yes it can import models of toolholders and use them in toolpath preview. As of yet, I don't believe that there is interference check for the toolholder, but in toolpath preview, you could visually detect a potential problem if you have a full model of your fixtures and the part. I expect this will evolve in the future***

15) Can OneCNC do batch processing (for example, run paths at night)?

*** Beats me If you have one process that requires that many hours to chew, I guess it would run all night Typically, I believe SMT allows for fast smooth toolpaths and within some toolpath parameter constraints, processing is quite rapid. You would have to try it (or get tech support to try it) on one of your files. But to answer your question, I don't think it does batch processing. ***

16) Does OneCNC have the ability to engrave with step-downs?

***SMT custom toolpath will cut any 2d geometry as if it were a projected toolpath onto any surface beneath it. It has an engrave amount (depth to cut into the model) and this can be varied at will.***

17) Does OneCNC have decent machine simulation with user configurable machines?

***I've seen several models of 4 and 5 axis fixtures that guys have created. It will rotate the 4th and 5th axis platters during toolpath preview. There is nothing stopping you from modelling more of your machine, although more entities on screen than necessary can slow down the manipulation speed, so simple machinery models are best. Any solid models on screen during an SMT toolpath creation/verification will be checked for tooltip interference.***

18)Does OneCNC have a "Cursor guide" that has an adjustable radius definition used as a guide for creating boundries etc. ?

***I'm not sure of how this feature works, but I would say no. A boundary can be offset of course, but once it is drawn and used in a process, that boundary (even if later deleted) is still remembered in that process. It is a permanent relationship, and cannot be altered within the existing process. However, the flexible option exists within every process to work with the tool tangent to the inside or the outside of said boundary, or to ride it, tip-centered, on the boundary. ***

As a final note, the developer is very keen, and very involved in updating the program. User feedback is monitored on the OneCNC site forum, and I would have to say that all difficulties that users have, are attended to, some sooner, and some later.
There is a plan being carried out which keeps things orderly and coordinated. Careful consideration is given to the introduction of new features to keep the interface easy to remember how to use.

[Dan B]

Thanks for the quick, and thorough, reply.

I just want to clarify the editing issue. Is this statement correct: "If I create a toolpath that is cutting too deep, I need to adjust the parameters and re-calculate."

I believe the answer will be yes from what you described. What we are used to in WorkNC is having a choice to fix these kind of issues either pre or post calculation. In other words, we can edit out the extra toolpaths by windowing around the unwanted paths and deleting them, the same way you would delete any geometry in a CAD software. Then the only re-calculation is to adjust retracts lead-ins etc. That takes only 3 or 4 seconds.

As far as the rest re-machining, WorkNC does handle this automatically. The only input needed is a reference tool size, so it can figure out the necessary overlaps.

It does seem like OneCNC is pretty complete. For multi-axis machining, a 3D stock model should be added, and holder collision checks should be on their enhancement list too.

I will keep an eye on this software and see how it develops.

Thanks again. This has been very helpful.

Dan

[HuFlungDung]

Dan
Are you meaning by "windowing around the unwanted paths and deleting them", actually somehow selecting regions of toolpath geometry out in the CAD window? I can hardly imagine that being the case, so I think you mean selecting an individual obsolete process from the 'group tree' shown here, and deleting it. Yes, of course. The individual processes can be deleted, dragged around in a new order, or even into a new group.

Typically, when ready to pull the trigger, you then post process one group at a time.

[Dan B]

Yes, in the CAD window. PowerMill has this too, but quite a bit limited compared to WorkNC (limited 2 years ago, I haven't looked at PM since)

You can isolate, delete, offset etc. using this method. It's quite handy, and we would miss it if it was gone! It allows the programmer to be "sloppy" with his set-up, knowing he can tweak the path in later in a matter of seconds. Of course if you take the time to do it right to begin with, editing is minimal if any.

However, when time is money, the quickest way is the best way.

Dan

[HuFlungDung]

I should add, we do not generally work with a backplotted toolpath at all. The toolpath information is created within each process's parameters at all times.

This may make it difficult to 'ultra tweak' a toolpath, but it results in safe, crash free programming as well.

You could under somewhat unusual circumstances I suppose, take and backplot a toolpath, then go in and modify it, then make a new process up using a stock path such as "Cut chain, variable Z" to machine the backplot.

This would take a lot of careful work, and the only proof of tool/machine/part safety would be your watchful eye during simulation or toolpath preview. Simulation should still warn of gouging, or visually demonstrate the tool destroying the part , so that is why I would say that this method is seldom used.

[Dan B]

I think we are speaking two different languages!

The graphics in WorkNC is created before post-processing, so the edits are part of the CL-APT creation, not tweaking G-code after the fact. When you do post in WorkNC, all retracts, gouges etc have been corrected. There is no risk.

I guess after using WorkNC for 12 years, it just seems like the right way of doing it.

Maybe I'm that "old dog" you hear so much about?


Dan

[HuFlungDung]

Dan,
I think you've hit the nail on the head.

Did you ask the guys in Florida if they would offer a 30 day dongle to you? I think that for serious inquiries, they might make the effort. They know full well that the users have to be satisfied with how the product actually works in the hands of the user, despite all the horn-blowing that I, or anyone else may do.

I know that some users can get more out of a given software product than others can, it is largely dependent on their background and expectations. The 'burden of learning' in OneCNC is reasonably low, that is one of its prime appeals. Even in the hands of the inexperienced, they can still 'make something' almost right away, whereas expert machinists can do wonders with it, and they're all looking at the same windows

[Dan B]

I have been corresponding with OneCNC in Florida, and they indicated that they don't do the 30 day demo thing, but it was not completely out of the question.

Honestly, I don't want to do that quite yet. Once they add simultaneous 5-axis I will take a harder look at this software. I'm not rushing into anything, as my decision will involve the purchase of 6 to 8 seats of software, and I will have to prove ROI.

On Tuesday I will be getting an in-house demo of HyperMill, and I want to look at UG too.

I'm hoping to drag this out for a while.

Dan