Mastercam

[Steven Craig]

I have a friend who is milling guitar necks for me using MasterCam. He said he would give me the MasterCam files. Can I use these files with the ShopBot?
Thanks

[dale]

Hi Steven:

You can BUT:
Depending on what post processor was used a little editing will have to be done. Mastercam will post a lot of code at the beginning of the program that is not needed by shopbot. Near the top of the program is a line referred to as the "Safety Block" It will include G40,G80,G49 etc. This line will have to be removed. If it contains G90, keep that code.
CNC machines use fixture offsets to tell the control where the origin of the part is. If the program you have contains "G54" near the third line, this code needs to be removed. This line will also contain the spindle speed. Remove Sxxx but keem the "M03 if you have a relay to turn on the router.Also, keep the x and y locations on that line. The next line will contain the code for setting the height offset for that tool. Remove "G43" and the "H" value from that line. If any drill cycles were used, "G98" or "G99" will have to be removed from the offending lines.
One very important thing to consider is G02 or G03. The G-code converter will only convert arcs if their midifiers are I & J. (Check with Bruce Clarke on this) If you have arcs with "r" as a modifier, The NCI file will have to be re-posted through Mastercam using a different post.
I hope this helps. If you have any trouble send me the files and I will see what I can do.
Good Luck
Dale

[waynesutter]

Depending on the complexity of the file you may be able to use the export function of Mastercam to write a DXF file. You can use line color on the geometry file to determine depth. Then use the FC command to convert the file to SBP format. I just created a complex part in Mastercam Version 7.1 and used the procedure above to convert and run it. It worked flawless!

Depending on the version of mastercam you have also. Posts for Mastercam can be very complicated but they are the key to successful file conversion. I teach Mastercam at a local community college and may also be able to help you. I have the manual for Mastercam Post editing and I am just now exploring the subtelties of creating a Mastercam post for the Shopbot. I suspect that I can edit one of the generic simple posts susch as the one designed for the DYNA 2936 controller. Perhaps your friend could try one of these posts for you. i will repost to this forum after I have determined the optimum post for the Shopbot and any changes needed.

Wayne

[waynesutter]

I have spent some time working on the best Mastercam post for use with Shopbot. There was a new basic post released last year and I do not think it has had wide distribution, I got it from my Mastercam dealer. The file is called MPBASIC.PST and I can send it to anyone that wants it. I ran a file that had a series of simple curves, lines and plunges and the Shopbot conversion from Mastercam .NC file was flawless and quick. If anyone is interested e-mail me. I am still working on this and I want to convert some more complicated files before I deem it done but it is very encouraging.

I love my new shopbpot!

[stevel]

I have written a post processor for Mastercam that will output a .SBP file. It outputs Shopbot M & J codes along with JS & MS codes with an optional SO,1,1 & SO,1,0 switch code. It will work with Mastercam Mill 7.2c and Mill 8.x. If you would like a copy of the post please email me. I want to thank Wayne Sutter for helping me test the post and for his input.

Steve Landkamer

[sutter@iinet.com]

I have used Steve's new Mastercam post and he deserves acolades for a great job. The post puts out native code for the shopbot directly to an sbp file. For anyone interested, Mastercam offeres educational prices for teachers and students that make this program a great deal. You can contact your local Mastercam dealer. they have separate dealers for education versus commercial so they may have to refer you to the correct dealer. Also many community colleges have copies and offer classes. I have taught some of the introductory seminars for Mastercam at the college I teach at.

[srwtlc]

Is Mastercam something that would be a good investment for a ShopBotter. I know it is highly acclaimed and I might be able to get a good deal on v8.1. Any opinions? Recommendations.

Scott

[rgengrave@aol.com]

Mastercan is nice to have but not for the price,you will find you can get 2 or 3 others that will fit all your needs for the same cost for Mastercam + be able to do others things too.

I have tried

Mastercam
Artcam
Milwizard
Casmate Pro
Signlab
Autocad
Turbocad
Vector
Rhino
Rams 3D
Coreldraw
and dozens of others only to find not 1 will do it all
After 4 years of playing around with them I found it to be simple just to use more then 1 program to make my files.

If you can get Mastercam at a real good deal then go for it, or check around and see what programs you can buy for the same price.

Just my 2 cents.

Ron V

[stevel]

Scott,
Mastercam is a fully complemented CAD/CAM package, all levels of Mastercam have 3D drawing capabilities and milling options from 2 1/2D through multi-axis milling. Mastercam is coming out with a Router product. Mastercam Router will have three levels of functionality and pricing. Buy what you need today and move up to the other levels when you need it.

I have been beta testing the Mastercam Router package and it has features that the Mastercam Mill packages don't have. The Mastercam Mill packages are geared to the metal working industry and the new Router packages are geared toward woodworking and plastics industry using routers. They have included some great features to name a few: Tabs, Nesting, Raster to Vector conversion, Door Creation.....etc.

Below is a link to the Mastercam Router information page.

http://www.mastercam.com/Products/V8Router/V8Router.htm

Mastercam has allot of flexibility in their Milling packages and the same concept has been put into the Router package. There may be features in Mastercam that you won't use today but it is nice to know that the power is there when you need it. Mastercam can let you generate drawings and toolpaths very quickly, and it all so has the depth to let you tweak your toolpaths to do what you want it to do.

Ron V named some dog gone good drawing packages in the list of products he has used. He all so listed some good CAM programs there all so. Some products are geared to a specific industry i.e. Signlab. If you are doing specific work you will want to find a package geared toward what you are doing. If you are going to be doing job shop kind of work you will need a "Swiss Army Knife" kind of package. In my opinion Mastercam can fit that bill. It is not a cheap package but it has the depth that you need for today and tomorrow.

That is my 47 cents worth.

Steve L.

[slappy]

I found a mastercam post in the download section
under drivers/patches. I installed it and it's been running perfectly ever since. I made the necessary edits to the post to make it run like i wanted.

[stevel]

Slappy,
I was just wonering what changes you made to the post? I wrote the post last year for my needs and a few other users needs and I have been considering some other changes to the post and I would like to know what other folks are looking for in the post.
Thanks,
Steve L

[Tulemaker@aol.com]

Hi,

I've been running Surfcam for many years and would like to use it making files for use on a shopbot. I'm familiar with customizing the post processer to work with other machinery thatn the Hass machining centers I also use. Can you give me a few parameter suggestions for customize the post so that it outputs a file shopbot can use directly or will I need to run it through a converter program?

Thanks,
Don Zacher

[oig01@hotmail.com]

My company has a allen bradley 9/230 with a cnc controller v1.0. The operators computer has crashed and we have lost the post. We are using mastercam 8.1 MILL. I have a generic post AB9230.PST but I need to modifiy it to get it to work on the waterjet ( manufactured by Flow international corp) I get a "NO FEEDRATE PROGRAMMEDED" error. There is a feedrate on our .nc file so I dont know what is wrong. I need a post for this waterjet.

Help!!

orlando
it technician
www.gusmercellulo.com (http://www.gusmercellulo.com)

[stevel]

Orlando,
If you contact your local Mastercam Dealer they should be able to help you out. I looked at your company web site so I am not sure if you are in NJ or CA. You can go to the Mastercam Dealer Locator (http://www.mastercam.com/ResellerLocator/us.asp)
to locate your dealer.

Steve

[simon]

I have just downloaded the trial version of Rhino, and I quite like it.
I would like to know if there are any modules available that can translate Rhino's output directly into shopbot code without having to open it into vector or something else. (Which kind of defeats the object of getting another program, since I currently do everything in Illustrator, and then Vector for depth and code.