Official Luthiers Forum!

There's nothing to take a screen shot of really. There is a button on the main screen labeled "save to kb" and another "load from kb". If you have something you like, you save it. If you need something you've done before, you simply load it. When you load it, it shows up as a machining tree without any geometry selected but all of the parameters for each machining operation are preserved from what you saved.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

I could be mistaken, but I don't think MadCam has an option to save toolpaths that way. At least I've never found a way to do it. MadCam saves its tree as layers within a Rhino model, and it seems to save its toolpaths as specific vectors along with a limited amount of related metadata for G code generation rather than as parameters that could be reused with a different model.

The only real issue I've had with MadCam is that it I haven't found a way to identify exactly what my parameters were when I generated my toolpaths if I come back to the model later on. It's not a deal breaker, but it requires me to keep a log book outside of Rhino to allow me to duplicate a machining plan. That's probably the issue Andy is referring to....

Of course, I could have missed something big here!

Dave

Yes, that's exactly the issue I was referring to and I think it was even one of your posts that brought it to my attention. It also brings up another question - if you make a change to a geometry of some sort, do you have to start from scratch or can you simply hit regenerate and boom, you're done?

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

You start from scratch (at least I do--again, I might be missing something). Like Rhino, MadCam isn't parametric--it's driven by the vectors that are present at the time of generation...

BUT, I have to say that starting from scratch doesn't take very long and isn't hard to do. The CAM process start to finish on something like an archtop guitar plate takes me maybe 5 minutes or less within MadCam. Not too bad.

Dave

I suspect to get to the bottom of it we'd need both packages open and running on the same machine. It's not the simple projects that are the issue, it's the complicated ones that are the big deal. I imagine that at least some of the info in MadCAM is re-useable.

e.g. I'm doing a solid body guitar right now that has 12 to 15 operations per side to get it right - roughing, drilling, pocketing, engraving surfacing etc. with all sorts of different bits, different containment sketches etc. etc….

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Yep, I agree. I would imagine that on a project like that solid body a person could tweek the design here and there and not be forced to re-do all of the toolpaths. If you changed the profile of the body, for instance, you probably wouldn't have to change the pocketing or drilling toolpaths that might not be dependent on the profile, but roughing, planar and z level paths would have to be redone in order to get it right.

Any information saved with the tool is definitely re-useable, but that's fairly limited info.

I think it's probably in the same category as the whole ATC question. If you're not doing a lot of design tweeking and not in a high-production mode, it's not as big a PITA as it would be in a higher production/multiple design variant environment. For what I do, I don't mind changing tools manually or re-doing toolpaths from scratch, even with complicated projects. But I am not in a high volume or variety situation, and a few minutes doesn't affect my bottom line. My outlook would be very different if I were! And, of course, there may be an easy way around all of this in MadCam that I haven't yet discovered....

Dave

Are you guys referring to this type file?




madCAM report:
Created on: 1/22/2014 10:14:44 PM

=========== Programmer notes ============

Programmed by: ADMIN-PC
Maximum Tool Length:
Approximate work piece dimensions: L=33.61; W=4.98; H=2.9

=========== Toolpath Specifics ============

Tool: T150 ( D0.500_L3.000 ) BALL_END_0,5
Path: Planar
Path: Zlevels

============= Code ==============

File successfully written as C:\Users\Mike\Desktop\KBR-LS.txt
Post Processor:C:\ProgramData\5XCNC\madCAM\5.0\Post Processors\Mach_3_Inch.txt

Tool changes: not specified in post processor
Rapid traverses: not specified in post processor
Cut in material: 23 minutes 32 seconds

Total machining time: 23 minutes 32 seconds

I can't speak for Andy, but what I was talking about was more of a template that could be reloaded containing all of the toolpaths along with any parameters that went along with the toolpath. This could then be reassigned to a different model. Essentially replicating what you had done earlier in terms of toolpaths, but on a different design.

Dave

Dave that might be possible with a much higher end software, but I don't think it is gonna happen for the lower end stuff like Madcam and VM.

Now I am not trying to be difficult here, but asking this out of curiosity. How much time do you think that would save over clicking the icons necessary to build the file in Madcam. It takes time to type in the parameters into the templates. My main question though, is how in the world is a piece of software going to be able to apply tool paths from one geometric model to another without having to recalculate, and if it has to recalculate, what time has been saved?

Mike

Turmite,

What they are talking about in Rhinocam or VM ...we have the ability to save a library with tool paths already established as far as direction, speeds , feeds, tool used, lead in lead out, etc......... For instance on a guitar neck we use regions extensively but from one different style neck to another we don't change the basic regions ( usually size and placement changes ) nor do we change the speed cut etc. provided we set all the regions up with the same general concept....... We typcially will use a 2D box for the region on various necks that are similar...... say a Martin Style 1 to a OOOO are all the same basic neck. We usually place the same general region at the heel, barrel, peghead etc. The regions define the area the toolpath is to work in and we usually do this at the bottom of the parts....... ( it will also work at the top but I seem to be able in my mind to deal with it better at the bottom.) When we are toolpathing a new neck we then define new boxes or regions and we simply pull up the library for say MS necks and select each region as the area requires and regenerate having only selected the region and not having to do all the detail things again.......... it is much faster than having to specify everthing for a typical cut once the same basic regions are established.

We have both programs ( Rhiocam Pro 2014 and Madcam 5 Xtra ) and typically we don't use Madcam for this kind of operation but I will look tomorrow for what you guys are asking about.

Blessings,

Kevin

Yes Dave and Kevin, that's exactly what I'm talking about and it's an extremely useful feature. It's late so I won't elaborate on Mike's question tonight but the time savings is very significant. I can walk away after I hit regenerate. Filling in the 10 to 20 or so parameters for each machining operation of 10 machining operations over all is a big deal.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

That was my point a little earlier--for me, it's no big deal at all. It doesn't take a lot of time, isn't difficult to do, and a little time doesn't mean much to me anyway. For guys who are making lots of complicated custom parts, and for a living, I can see the benefit though. I'm quite happy with MadCam.

Dave

Now that I have a little more time…

First of all, I'm not trying to knock MadCAM at all. I use SolidWorks as my main CAD package so that right there is the deal breaker for me. From everything I've heard and read, it's a very capable CAM package.

To elaborate on your question though - the time savings can be significant for a couple of reasons. First - there's no need to keep a log book anymore. Because the parameters are stored with the file, you can always go back and refer to and old strategy and get your settings.

Selecting geometry for a machining operation is less than half of the time necessary for the operation. Setting all of the feeds/speeds, entry/exit etc. is usually more than half of the time spent creating a machining operation.

Also, any time manual entry is involved, there's the chance of fat fingering a parameter or something like that. At least one time I accidentally entered 1800rpm for my spindle speed instead of 18000!

Kevin gave a great example with the neck. I'll give another. I make a lot of bridges for people. Although they look very different, the basic machining operations are the same:

Rough cut the end grain of the wings leaving behind a little bit of stock
Finish cut the end grain
Rough cut the front and back profiles
finish cut the front and back
engrave certain areas for protection against tearout
3D surfacing
Saddle slotting
pin drilling
chamfering

So here we have 9 operations that each have a bunch of parameters to enter in addition to selecting geometry. Not having to re-enter parameters saves not only about 50% of your time, it also to a degree error proofs the creation of the tool paths since you're loading a machining strategy from a part you've most likely proven out already.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Andy I have never even considered you bashing Madcam. I am here to learn and have been in contact with Joakim the writer of Madcam and he told me this is already possible within Madcam, but I am waiting on a Skype from him so we can discuss this in depth. I am trying to learn all I can because down the road, it will help someone else.

Ok, so you have the 9 operations listed that have to be done. Do you just plug in the new geometry of the new model or version, and the software automatically applies the cutter, speeds, offsets, regions, clipping planes, feed direction etc to the new model? You just click a button and have a new tool path on a new model? If so, then yes, this is something we need to do, because if VM can offer it, we have to!

Mike

Hi Mike,

Yes, with the exception of regions, everything else you write is possible in VM using the Knowledge Base feature. Regions are tied to geometry and that's the only thing that's not saved when you save something to a knowledge base.

Also, just in normal use in a project, at least with SolidWorks, when you tweak a model, regenerating tool paths is just a click of a button. The exception is that if you delete entities and replace them, you do have to re-select. This might be a fundamental difference between Rhino and SW though as you can make drastic changes to models simply by tweaking dimensions without deleting or adding any entities.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Hi Andy,

Isn't amazing what you can learn when trying? I just spent about an hour on skype with Joakim in Sweden and to my surprise, not only can Madcam do what you are describing, it can do it a couple of different ways, one manual and the other automajically through a script.

He is doing a video for me to post so that I don't have to try to explain it in my feeble ways!

Vid should be ready sometime tomorrow. Thank you for posing the original question which got me involved in trying to figure out what in the world you were talking about. That said, Joakim told me that this will also be a win/win for me in my product
(non guitar) line. Needless to say, I was shocked. He did tell me that Madcam has much built into it that has not yet been revealed but they are nearly finished with a new website that will be filled with videos showing many of these hidden nuggets!

Again, thank you for the "push" as the original poster said.

Mike

I'll be waiting for this movie Mikey!! Sounds like Joakim is well and active!.

Thanks
Shane

_________________
Canada

Yeah Mike--Thanks! I've always known that there's a lot about MadCam that I don't know....

I look forward to seeing what Joakim has to show!

Dave

Is it available for all versions of Madcam or just the higher ones, ...Mike?

_________________
Ken

Good deal! I need you guys to keep Mecsoft on their toes!

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Well I did not get the video today, but will go ahead and try to explain this without messing it up. Within Rhino you have the ability to save the commands in the command line during a complete string of work, and as it relates to Madcam, it will save each step you use to build the tool paths. You can save that file from Rhino as a txt file or as Joakim said, it is easiest to build a script to do the same thing, only automatically. When you have made the tool paths and saved the file, save it as a particular strategy. Pull up a new model that is similar but not the same, copy and paste the saved file into the command line and the tool paths will be created on the new model!

For those of you that know me, you know my main business is building rifle stocks and pistol grips for competition shooters. Joakim told me yesterday that this would work the same for my products as it would for guitar parts. I found that very enticing.

We are suppose to do an JoinMe.com training early this next week with him teaching me how to set this up, use it and the ability to help those that want to apply it.

I will post the video as soon as I have it.

Mike

Thanks Mike--I'll give it a shot today.


Update: I tried saving and reloading the Rhino commands, and there's apparently more to it than that. It definitely takes some editing of the text file before Rhino will do anything with it--there might be an easy way to deal with it, but I'm betting that turning it into script is going to be the better option. After editing the file, I can get it to prompt me for a cutter and a box, but it doesn't like to accept the parameters as they were entered previously. I'm sure it's something simple that I don't know how to do yet.



Dave

Thanks Dave,

Well you need to remember I was trying to recount what he told me from memory.....and that might not be such a good idea either. Hopefully the vid will be here soon.

Mike

I understand--if your memory is anything like mine, you did darned well to even remember what we were talking about! Doesn't seem to get any better as I get older either...

Thanks for digging on this one!

Dave

Guys I just got off skype with Joakim and he is working on the video now. Later then evening and I will post it.

Mike