Go to Post FIRST is about family, making new friendships, belonging somewhere, doing something you love, and finding out what your real love is in life, so when you're old and wrinkly you can look back at high school and say "This is when I found myself." - Winged Wonder [more]
Home
Go Back   Chief Delphi > Technical > CAD
CD-Media   CD-Spy  
portal register members calendar search Today's Posts Mark Forums Read FAQ rules

 
Reply
Thread Tools Rating: Thread Rating: 2 votes, 5.00 average. Display Modes
  #1   Spotlight this post!  
Unread 02-08-2011, 11:00
docdavies's Avatar
docdavies docdavies is offline
Doc Davies
FRC #0346 (RoboHawks)
Team Role: Mentor
 
Join Date: Mar 2010
Rookie Year: 1998
Location: Richmond, VA
Posts: 70
docdavies is an unknown quantity at this point
Autodesk Inverter Pro 2012 - MasterCAM - CNC

By some miracle, our school was able to obtain a CNC machine which is intended to be used in classroom situations and by our FIRST Robotics Team. I was involved in it's uncrating, set up, and about a 20 minute "Here's how it works" session from a technician that just really wanted to go home at 6:30 PM. We intend to rectify that.

I kept asking, "Can we go from Inventor Pro to a finished part". Answer..."yes of course you can, with a translator..." and what boiled down to "A lot of luck".

In the long run, no matter how many return trips and brow beating we do, I don't think he's going to be much help.

So, has anyone else out there gone through this? Can you point out some tutorials or related info?
Reply With Quote
  #2   Spotlight this post!  
Unread 02-08-2011, 22:39
sanddrag sanddrag is offline
On to my 16th year in FRC
FRC #0696 (Circuit Breakers)
Team Role: Teacher
 
Join Date: Jul 2002
Rookie Year: 2002
Location: Glendale, CA
Posts: 8,519
sanddrag has a reputation beyond reputesanddrag has a reputation beyond reputesanddrag has a reputation beyond reputesanddrag has a reputation beyond reputesanddrag has a reputation beyond reputesanddrag has a reputation beyond reputesanddrag has a reputation beyond reputesanddrag has a reputation beyond reputesanddrag has a reputation beyond reputesanddrag has a reputation beyond reputesanddrag has a reputation beyond repute
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

I don't know what software or controller your machine uses but chances are it runs standard G-code. What I usually do is create a 2D .idw drawing in Inventor (in 1:1 scale of course) and then save that as a DXF. I then open the DXF in MasterCAM X and create the toolpaths, export the G-code, and load it into the machine. I suppose it's also possible to import a 3D model into MasterCAM but I don't do it that way for the simple stuff I do.

Do you have MasterCAM? If not, I'd recommend it. There are alternatives but in my opinion they don't compare.
__________________
Teacher/Engineer/Machinist - Team 696 Circuit Breakers, 2011 - Present
Mentor/Engineer/Machinist, Team 968 RAWC, 2007-2010
Technical Mentor, Team 696 Circuit Breakers, 2005-2007
Student Mechanical Leader and Driver, Team 696 Circuit Breakers, 2002-2004
Reply With Quote
  #3   Spotlight this post!  
Unread 03-08-2011, 15:40
docdavies's Avatar
docdavies docdavies is offline
Doc Davies
FRC #0346 (RoboHawks)
Team Role: Mentor
 
Join Date: Mar 2010
Rookie Year: 1998
Location: Richmond, VA
Posts: 70
docdavies is an unknown quantity at this point
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Sanddrag,

The "system" came with MasterCAM x5 (?). During the hocus-pokeus set up demonstration, I thought I saw the MasterCAM software guide the production of a "part". Problem was, fingers were flying, keys were pounding, mice were zooming and it was hard to tell what was happening. The installer had taken 6 hr to get it going and just really wanted to go home.

But we did ask about Gcode, and were able (actually we had to, to change to a bit we had that the machine didn't know about) edit it. But the whole process was not pretty.

In a nut shell, we have Autodesk Inventor Pro 2012 (and we've become much better with it), MasterCAM x5 (and supposedly all the translators and libraries) and the following machine....

http://www.techno-isel.com/Education1/Patriot.htm


So, are there tutorials on how to go from Inventor, where we currently do all our designs, to finished part?

Thanks for your patience all!
Doc

Last edited by docdavies : 03-08-2011 at 15:42.
Reply With Quote
  #4   Spotlight this post!  
Unread 03-08-2011, 16:24
R.C.'s Avatar
R.C. R.C. is offline
2017... Oooh Kill em, Swerve!
AKA: Owner, WestCoast Products
FRC #1323 (MadTown Robotics)
Team Role: Engineer
 
Join Date: Feb 2008
Rookie Year: 2006
Location: Madera, CA
Posts: 2,186
R.C. has a reputation beyond reputeR.C. has a reputation beyond reputeR.C. has a reputation beyond reputeR.C. has a reputation beyond reputeR.C. has a reputation beyond reputeR.C. has a reputation beyond reputeR.C. has a reputation beyond reputeR.C. has a reputation beyond reputeR.C. has a reputation beyond reputeR.C. has a reputation beyond reputeR.C. has a reputation beyond repute
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Doc,

I sent you an email, I can for sure help you with this. Our rep was very helpful when we started. Who did you buy this through?

-RC
__________________
R.C.
Owner, WestCoast Products || Twitter
MadTown Robotics Team 1323
Reply With Quote
  #5   Spotlight this post!  
Unread 04-08-2011, 00:17
Jeff 801's Avatar
Jeff 801 Jeff 801 is offline
Registered User
no team
Team Role: Alumni
 
Join Date: Jun 2006
Rookie Year: 2004
Location: Florida
Posts: 346
Jeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond repute
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

I personally have used Autodesk Inventer 2009 with MasterCAM 9 and a CNC.

Basically what I do is I create the part as a 3d model (.ipt) even if it is just going to be a plate that will be machined. From there I create a drawing (.idw) at 1:1 scale and save it as a DXF. MasterCAM is able to import the DXF directly and from there I create the tool paths that are needed. To finish up in MasterCAM I export the tool paths into G-Code (also called post processing) and because the machine I work with does not have an automatic tool changer I post each tool of the program to a separate G-code file.

I have played with MasterCAM x5 and it does all the same things that 9 can do its just the menus are different. The same goes for Inventor 2009 just has a different layout than 2012 (and its more stable IMHO)

Hopefully that explains it a little more.
Reply With Quote
  #6   Spotlight this post!  
Unread 04-08-2011, 01:40
Cory's Avatar
Cory Cory is offline
Registered User
AKA: Cory McBride
FRC #0254 (The Cheesy Poofs)
Team Role: Engineer
 
Join Date: May 2002
Rookie Year: 2001
Location: Redwood City, CA
Posts: 6,823
Cory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond repute
Send a message via AIM to Cory
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Quote:
Originally Posted by Jeff 801 View Post
I personally have used Autodesk Inventer 2009 with MasterCAM 9 and a CNC.

Basically what I do is I create the part as a 3d model (.ipt) even if it is just going to be a plate that will be machined. From there I create a drawing (.idw) at 1:1 scale and save it as a DXF. MasterCAM is able to import the DXF directly and from there I create the tool paths that are needed. To finish up in MasterCAM I export the tool paths into G-Code (also called post processing) and because the machine I work with does not have an automatic tool changer I post each tool of the program to a separate G-code file.
Why do you bother with the extra step of converting to .idw and .dxf when you could just save as a STEP, IGES, or Parasolid file and go directly to MasterCAM with that? Does 9 not allow those file formats? I know X through X5 allows nearly every format imaginable, with the caveat that you need to update frequently if you want to stick with native Inventor/Solidworks/ProE files that were created with the newest model year.

Also, depending how your machine works, you might be able to save time by posting out all your tools in one program, with a M00 command between each one. This will force the machine to always stop when the M00 is reached, allowing you to change tools, and then start up where you left off and machine with the next tool.
__________________
2001-2004: Team 100
2006-Present: Team 254
Reply With Quote
  #7   Spotlight this post!  
Unread 04-08-2011, 01:50
Jeff 801's Avatar
Jeff 801 Jeff 801 is offline
Registered User
no team
Team Role: Alumni
 
Join Date: Jun 2006
Rookie Year: 2004
Location: Florida
Posts: 346
Jeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond reputeJeff 801 has a reputation beyond repute
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Quote:
Originally Posted by Cory View Post
Why do you bother with the extra step of converting to .idw and .dxf when you could just save as a STEP, IGES, or Parasolid file and go directly to MasterCAM with that? Does 9 not allow those file formats? I know X through X5 allows nearly every format imaginable, with the caveat that you need to update frequently if you want to stick with native Inventor/Solidworks/ProE files that were created with the newest model year.

Also, depending how your machine works, you might be able to save time by posting out all your tools in one program, with a M00 command between each one. This will force the machine to always stop when the M00 is reached, allowing you to change tools, and then start up where you left off and machine with the next tool.
MasterCAM 9 allows those formats I just like to work with a 2d model in MasterCAM because its simpler for me just a personal preference and I just have not gotten around to learning the new interface of x-x5 (I learned mastercam 5 years ago ish and just have not kept up to date)
Reply With Quote
  #8   Spotlight this post!  
Unread 04-08-2011, 10:18
docdavies's Avatar
docdavies docdavies is offline
Doc Davies
FRC #0346 (RoboHawks)
Team Role: Mentor
 
Join Date: Mar 2010
Rookie Year: 1998
Location: Richmond, VA
Posts: 70
docdavies is an unknown quantity at this point
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Folks,

Everything you are suggesting seems great. But please remember, you're like a nuclear physicist attempting to explain a Thorium reactor to a 3 year old. We are just not working off the same knowledge base....from my side, I really need to get up to speed! So, can you suggest any GOOD books or on-line tutorials that would at least teach me to speak the same language, and have concept of how things SHOULD happen, even if I don't currently know how they do happen?

On slightly more depressing note, the more I look into the actual CNC machine we have (link provided above), it looks more like it's meant to be a teaching machine for use on wood, plastic and maybe "soft" metals. And not a machine that's going to be suited for our robotics builds.

Thanks,
Doc
Reply With Quote
  #9   Spotlight this post!  
Unread 24-08-2011, 06:52
docdavies's Avatar
docdavies docdavies is offline
Doc Davies
FRC #0346 (RoboHawks)
Team Role: Mentor
 
Join Date: Mar 2010
Rookie Year: 1998
Location: Richmond, VA
Posts: 70
docdavies is an unknown quantity at this point
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Well, progress. My younger son, who's just started FRC last year as a freshman, took an Inventor Pro File that had been graciously converted by RC to run under MasterCAM, and got it to run in the machine on a chunk of wood. Following several suggestions gleaned on-line we're picking up some carpet tape and will try to cut the piece out of aluminum during a Sat. summer build session.

I'll let you know how that goes.

Thanks again to the FIRST community for all your help.....
Doc
Reply With Quote
  #10   Spotlight this post!  
Unread 27-08-2011, 10:56
DonRotolo's Avatar
DonRotolo DonRotolo is offline
Back to humble
FRC #0832
Team Role: Mentor
 
Join Date: Jan 2005
Rookie Year: 2005
Location: Atlanta GA
Posts: 7,019
DonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond reputeDonRotolo has a reputation beyond repute
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Just a suggestion: When practicing, you may want to consider using styrofoam (the pink or blue stuff sold as Home Depot/Lowe's) or, even better, machining wax (google it, several online suppliers). Both are soft, inexpensive materials that will allow you to machine things without damage if the tool decided to make a cut it can't. Aluminum is less forgiving. Bonus for the wax: Melt the chips into a cake pan and you have a new block.
__________________

I am N2IRZ - What's your callsign?
Reply With Quote
  #11   Spotlight this post!  
Unread 30-08-2011, 09:42
docdavies's Avatar
docdavies docdavies is offline
Doc Davies
FRC #0346 (RoboHawks)
Team Role: Mentor
 
Join Date: Mar 2010
Rookie Year: 1998
Location: Richmond, VA
Posts: 70
docdavies is an unknown quantity at this point
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Don --> I like it! Since I've been spending a lot of time at Home Depot getting generators, extension cords, gas cans and such....I'll pick some up on my NEXT visit, which will probably be today.
Reply With Quote
  #12   Spotlight this post!  
Unread 12-10-2011, 06:54
docdavies's Avatar
docdavies docdavies is offline
Doc Davies
FRC #0346 (RoboHawks)
Team Role: Mentor
 
Join Date: Mar 2010
Rookie Year: 1998
Location: Richmond, VA
Posts: 70
docdavies is an unknown quantity at this point
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Mixed progress. We have been able to manufacture parts out of Lauan Plywood and Lexan. Using 0.125 aluminum gives mixed results most likely due to technique and improperly setting the material in the software.

All of our attempts to go from an Inventor Pro 2012 part file (or any of the other extensions you can save it under) have been unsuccessful. We can open the file in Mastercam, but as we try to add toolpaths, we get error messages or it simply will not select the contours.

We have tried to install Mastercam Direct and Direct for Inventor, but have not had much luck there either.... And there is very little documentation on installation, configuration and use.

If you've had experience with this same situation and have found solutions, I'd love to discuss them with you.

Doc
Reply With Quote
  #13   Spotlight this post!  
Unread 12-10-2011, 10:21
Cory's Avatar
Cory Cory is offline
Registered User
AKA: Cory McBride
FRC #0254 (The Cheesy Poofs)
Team Role: Engineer
 
Join Date: May 2002
Rookie Year: 2001
Location: Redwood City, CA
Posts: 6,823
Cory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond repute
Send a message via AIM to Cory
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Quote:
Originally Posted by docdavies View Post
Mixed progress. We have been able to manufacture parts out of Lauan Plywood and Lexan. Using 0.125 aluminum gives mixed results most likely due to technique and improperly setting the material in the software.

All of our attempts to go from an Inventor Pro 2012 part file (or any of the other extensions you can save it under) have been unsuccessful. We can open the file in Mastercam, but as we try to add toolpaths, we get error messages or it simply will not select the contours.

We have tried to install Mastercam Direct and Direct for Inventor, but have not had much luck there either.... And there is very little documentation on installation, configuration and use.

If you've had experience with this same situation and have found solutions, I'd love to discuss them with you.

Doc
Doc,

What error message are you getting?
__________________
2001-2004: Team 100
2006-Present: Team 254
Reply With Quote
  #14   Spotlight this post!  
Unread 12-10-2011, 17:45
docdavies's Avatar
docdavies docdavies is offline
Doc Davies
FRC #0346 (RoboHawks)
Team Role: Mentor
 
Join Date: Mar 2010
Rookie Year: 1998
Location: Richmond, VA
Posts: 70
docdavies is an unknown quantity at this point
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Cory,

Got that part worked out. And can now do tool paths. The problem I have now is I apparently do not know how to set up the stock or the cutting depths. The bit starts cutting above the stock and only goes part way down. This is probably easy to fix, but I'm burnt out after today...tomorrows problem.

In any case, looks as if (after minor tweaking and continued learning) that we will be able to go directly from Inventor Pro 2012 to CNC machine. I'm happy about that...will go a long way to reduce a lot of our tedious machining.

Doc
Reply With Quote
  #15   Spotlight this post!  
Unread 12-10-2011, 22:33
Cory's Avatar
Cory Cory is offline
Registered User
AKA: Cory McBride
FRC #0254 (The Cheesy Poofs)
Team Role: Engineer
 
Join Date: May 2002
Rookie Year: 2001
Location: Redwood City, CA
Posts: 6,823
Cory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond reputeCory has a reputation beyond repute
Send a message via AIM to Cory
Re: Autodesk Inverter Pro 2012 - MasterCAM - CNC

Quote:
Originally Posted by docdavies View Post
Cory,

Got that part worked out. And can now do tool paths. The problem I have now is I apparently do not know how to set up the stock or the cutting depths. The bit starts cutting above the stock and only goes part way down. This is probably easy to fix, but I'm burnt out after today...tomorrows problem.

In any case, looks as if (after minor tweaking and continued learning) that we will be able to go directly from Inventor Pro 2012 to CNC machine. I'm happy about that...will go a long way to reduce a lot of our tedious machining.

Doc
Go into "properties" in the part tree on the left and then "stock setup". Ensure that your boundaries are set properly and your origin is located correctly. I like to turn on the "display wireframe" option to see this clearly. Make sure either the top or bottom face of your part is your stock zero (or the top of your stock, if you're machining out of a larger block. Just make sure you know where it is).

That should locate your stock properly. If you have problems and are using verify, click the little file folder on the verify box and select "use stock setup values". Sometimes it gets messed up here-particularly if you switch the stock part from rectangular to cylindrical.

I forget which tab it is in MasterCAM X5 as I know they changed it from previous revisions, but when entering an operation go to the parameters tab, or whichever one gets you to the depth/top of stock/retract fields.

Ensure that your top of stock shown is 0 if the top of your part is Z0. or whatever the distance is between the origin and the top of your stock. If you click the "top of stock" button it will take you to the model and allow you to select a face. This is my preferred method of depth selection for things like contours and pockets-much less opportunity to fat finger a number.

For depth you can do the same thing-click the button for depth, then click any feature that is the depth you want to machine to, or enter the depth manually.

Finally one thing I noticed that caused me many headaches in X5 is that by default all values are incremental. This is really stupid and a great way to break things really easily. Ensure that retract, top of stock, and depth are all set to absolute unless you really know what you're doing and have a reason to change them. I would go into the settings and change the default. If I had to bet I would guess this is your problem currently.

Hopefully that helps.
__________________
2001-2004: Team 100
2006-Present: Team 254
Reply With Quote
Reply


Thread Tools
Display Modes Rate This Thread
Rate This Thread:

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

vB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Forum Jump


All times are GMT -5. The time now is 11:05.

The Chief Delphi Forums are sponsored by Innovation First International, Inc.


Powered by vBulletin® Version 3.6.4
Copyright ©2000 - 2017, Jelsoft Enterprises Ltd.
Copyright © Chief Delphi