Autodesk Inverter Pro 2012 - MasterCAM - CNC

[docdavies]

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?

[sanddrag]

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.

[docdavies]

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

[R.C.]

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

[Jeff 801]

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.

[Cory]

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.

[Jeff 801]

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)

[docdavies]

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

[docdavies]

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

[DonRotolo]

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.

[docdavies]

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.

[docdavies]

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

[Cory]

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?

[docdavies]

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

[Cory]

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.

[docdavies]

Cory,

Everything you mentioned is spot on. Some of it I just figured out this morning. The absolute thing was driving me nuts for a while. Another problem I had is, when you extrude parts in Inventor, you have to be very careful as to whether you extrude in, out or from the middle of the 2D drawing as MasterCAM seems to pick the surface based on that plane.

The other depth settings you mentioned seem to be under Toolpath >> Parameters >> Linking Parameters. I had to play with that quite a bit this morning as well.

Thanks again,
Doc

[sanddrag]

Can a mod re-title this thread with the proper spelling of Inventor for future searching?