3D Prallel Milling Problem

[engr.adnan_pk]

i am using inventor HSM 2016. i use 1.5 ball nose to machies the following curvatures with 3D Parallel milling stratagy..Insted of doing parallel milling tool behaviour change to drilling in some points. how to overcome this problem? inventor file is attached.....

[makko74]

Hi,

Possibility Number 1:

Add the Top Surface to the Avoid/Touch Surfaces

Possibility Number 2.

Add the Top Surface to the Model Surfaces and on the Heights Tap - Top Height - Top Offset eg: -0.001mm

there are surely more Possibilitys.

mario

153

[engr.adnan_pk]

I Add the Top Surface to the Avoid/Touch Surfaces, but this will leave a step on top of the job.

[makko74]

Then try the second one

For comparison with possibility 1

mario

258

[engr.adnan_pk]

both are not working.....i checked

[makko74]

Sorry then i can not help. Your question was how to prevent drilling.

better you ask @Rob.Lockwood, Rob is a preeminent in this field, you can look here.

mario

292

[engr.adnan_pk]

second worked but after i add the top surface as model surface. i will check it on my VMC (ecoline Ecomill 1035 DMG Mori with Seimens 840d controller) and then tell you.......Thanks

[engr.adnan_pk]

what is the logic behind

Possibility Number 2.

Add the Top Surface to the Model Surfaces and on the Heights Tap - Top Height - Top Offset eg: -0.001mm

why by adding -.001 on top height top offset will stop tool to remain parallel.....?

[makko74]

I hope you understand my bad english, it may be better if someone with better knowledge of English explains.

You have just only selected Model surfaces and not the Setup Model, so HSM is only looking at this surfaces on toolpath calculation.

the tool path calculation is performed in tool direction between top height and bottom height but all selected surfaces in tool direction from Retract height down to Bottom Height are considered.

Top Face in your example is on zero, to take it into toolpath calculation you must select it and set the top height a little bit deeper (  -0.001 ) to prevent it from processing.

So HSM knows that it must take the surface into the toolpath calculation but must start with the toolpath calculation at -0.001mm.

mario

62

[engr.adnan_pk]

very helpful thanks

[makko74]

When it is not logic there are also the way with boundarys. ( Possibility Number 3: Many roads lead to Rome. )

Draw a large rectangle on a new sketch as outer boundary ( Large enough that the tool has space between part and rectangle )

take the Top Face as inner Boundary, processing is then between this boundarys.

no need for choose Model Surfaces, let your Avoid/Touch Surfaces how they are

Additional Offset >0, then there is a smoother transition to your Top surface

Now you can choose the best solution for you

mario

98