My company is looking moving into the world of model based machining (at least that's what we call it).  I've been charged with coming up with the process for generating the solid models we would send to our machine shops.  I'm struggling with how to determine what qualifies as a "good" model.  Any feedback would be appreciated.

 Thanks!

DOWEND

I can give some guidelines for developing correct model. May be you will find it useful. You can develop from it further.

Create sketch and use that for extrude or revolve operation. Don’t create sketch inside extrude or revolve features. For simplified models it is better to create sketch with in the features to reduce the file size.

Draw required profile to approximate shape, then fix the geometric constrains, and dimensions per reference drawing.

Dimension the sketch as similar to shown on the drawings.

Select / draw profile which has the maximum number of dimensions in it (i.e. to create cylinder, draw rectangle to ID, OD and height then revolve the profile to 360 deg., rather then draw 2 circles and extrude).

Avoid duplicate input dimensions, for this you can use the previous dimension expressions when you use second time. i.e to specify wall thk in for side, 1^st location specify the values and 2^nd and so specify the 1^st value reference.

While creating new sketch hide the previous sketch(s), to avoid any relations with them, unless you need for that.

Create holes using features hole and array (pattern). Avoid using sketch for producing the holes.

Use sketch primary lines or datum’s for dimensioning and positions the holes.

Create model surface exact to outer (for male thd) or inner (for female thd) diameter of the thread, when you want to create male straight or male or female taper threads.

Avoid fillets and rounds in sketch, unless those are going to play in the functional.

Create fillets and rounds as last features. This will help to suppress or delete them when you import model for FEA. Since chamfer and round will have problem in FEA meshing.

Use datum to trim the body where ever possible, rather then creating a sketch.

Create symmetric components one half and mirror the same, then create holes, threads and so on.

Use part copy function to create machining model. Don’t create casting and machining in one model or family of parts, which leads 3 model files for one cast and machining.

Identical shape components try to create thru family of parts.

Create models for the tabulated drawings using family of parts

Parts are to be created one feature at a time.  Sketches with multiple features are not to be used.  Simplifying the part this way will reduce errors when modify or update a model.

Sketches are to be fully constrained and check so that the right constraints were applied.

Parts will only be created using dimensions available on the print.  If sufficient information is not available on the print, dimensions maybe added to create the part to the shape.  These dimensions are to be created with the thought in mind that will update when you go for changes in the given dimensions.

Ensure the final model file does not have any suppressed features.

Do geometry inspection after completing the modeling.

Check the density value before calculating the mass properties

 Good Luck!

Thanks for the help!  I did have a couple of questions.

 First can you expand on what you mean by "Do geometry inspection after completing the modeling."?

Second how do you deal with resolved dimensions?

Third, do you use associative dimensioning only?

Dave D

By geometry I meant the angular surfaces, and those with complex machining like spherical or other contours and the external casting or forging surfaces. This can be verified by using the appropriate measure option of the S/W.

Always follow the pattern of dimensioning as given in the print unless otherwise the print itself is wrong. This should take care of your second and third question.

Thanks