'Disposable' Reference Surfaces in Toolpath

[rokahn]

I'm using SolidWorks to create models followed by MasterCam to create toolpaths for a vertical mill. I find that I frequently want the toolpath to create spurs/reference surfaces into one side so when flipped over, the spurs help the piece be located properly in the vise/fixture for the milling pass from the other side.

These spurs will either be removed by this second pass or by manual touch-up. That means the spurs are not part of the part and don't appear in the model...or at least not in the model that gets linked into the assembly.

I'd appreciate people's wisdom about how to create these spurs/reference surfaces:
1. Should I create the spurs in solidworks but suppress spur features when I use the part for assemblies?
2. Should I create a 'special' assembly combining the part and the spurs...then export the assembly solid to MasterCam?
3. Should I create a 'copied part' with the spurs in SolidWorks
4. Should I create the spurs in MasterCam (doesn't sound like a good idea)
5. Any other ways I'm not thinking of...

Thanks for your thoughts.

Rocky

 

[MadMango]

I think the easiest thing to do would be to create these spurs in a new configuration of your part, then you can Suppress them when you don't need them, but will always have them available in case you need to alter them. "The attempt and not the deed confounds us."

 

[Stoker]

1. This works well. The only exception is when you also have several other configurations of the part (for reasons other than machining). Unless you have a good naming scheme it may be confusing for others who need to work on the part, but for most instances this is the best option.

2. If you create an assembly, you have the added overhead of multiple part files. You also have to join the parts before exporting anyway - too much hassle.

3. You could use a derived part to hold the machining data. The base part would be in the final machined state and the derived part would have added features for the spurs and any other tooling features. If you have multiple machining operations all of this extra data is held in the derived part. There are a couple of advantages to this. First, the final part file does not have all this extra baggage - meaning any assemblies or drawings which reference the part will load faster. This benefit could be significant if you work with assembly drawings which contain a large number of machined parts. Also, the part file is easier to understand because all machining features are held in the derived part. The only drawback is that you have two part files.

4. I don't like modelling in MasterCAM. Even though they are trying to advertise it as an alternative to CAD systems like SWX I don't know many people who prefer to create parts inside MasterCAM instead of importing them.

5. I can't think of any. Your best choices are 1 and 3.

 

[rokahn]

I think Stoker has implicitly seconded MadMango's suggestion to use configurations to describe temporary machining features (though neither has specifically evaluated using suppressed features without configurations). Looks like configurations are the way to go--at least for assemblies with small numbers of parts.

 

[rocheey]

You didnt mention what version of mastercam you're using,
or if using surfaces/solids. Ideally, you'd want machining-related geometry to be on your CAM side, but MC doesnt have much of a remachining-of-stock type feature.

v7 and above *do* let you import non-orthagonal models
in the toolpath verification process, but this is an extra feature. That would probably be the easist way to go, if you have that feature enabled in masterCAM