Autodesk Inverter Pro 2012 - MasterCAM - CNC

[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]

Originally Posted by 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

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]

Originally Posted by 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

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?