Cavity milling cutter path

[LMTDCS]

When milling a u channel (any cavity) that has holes thru the bottom or cutouts on the side walls, is it possible to
have the cutter path ignore these features with out hiding the feature or creating a new mfg solid?? As an old Ideas user we had the option of ignoring surfaces when milling. We want a smooth liner cutter path vs one that recognizes every opening and avoids or follows these openings. I have attached a .tiff file showing what we dont want!

Thanks in advance
Chris
L&M Tool

 

[wmalan]

Are you using a Blank solid? It looks like there's no Blank solid which causes to the tool to cut only the part faces. CavityMill works best with a Blank solid. The other benefit is you have as-cut stock for the subsequent operations.

Create a simple block of the channel cut area for Blank. Select only the Part faces you want to cut. Set the channel floor as bottom. The tool will now cross those holes and notches (ignoring them).

--
Bill

 

[wmalan]

I forgot to add, do NOT select Cut Areas or Wall Cleanup. As they will direct the tool to those areas.

--
Bill

 

[markrief]

If you pick the faces of the slot as cut area, the closed holes should be ignored. You may have to set the small area avoidance.

For the open slots, take a look at the options for extending cut area.

If you can not get what you want using the options in cavity milling, you may need to prep the model first. There are several options on the geometry tool bar in CAM, such as Patch Openeings and Trim/Extend, that should help you.


Mark Rief
Product Manager
Siemens PLM

 

[LMTDCS]

Thank you for the input. You all verified what I thought.
I will have to create simple solids to close the area up. I was hoping for a feature like in Ideas of just ingnoring the unwanted areas.

Chris

 

[Denim]

Noob question for the guru's coming up..

If you create new solids or sheets to prep the model, you will need to include these in your part geometry in order to be able to select them as cut areas, correct?

So if your operation is inheriting part geometry from a workpiece, then the new solids needs to be included in the workpiece, and then you have to create a new workpiece without the extra geometry to be able to machine the "covered up" regions later on?

I have done this before, but ended up with a very complicated and messy geometry setup with multiple workpieces and MCS's since the parts had to be machined in multiple orientations on a 5-axis machine.

Am I missing something or is it really that complicated?

/E

 

[wmalan]

Denim,

My own "style" of programming is to not include the Part in the Workpiece definition. Perhaps only the initial Stock. This allows me to select individual part features in each operation without affecting the workpiece. The other issue is it can really slow down your system to have say a whole solid processed at every operation. Some jobs may lend themselves to using the whole part solid but usually not for me (large airframe models). The down side is Compare in Toolpath Verify will not show gouges or thicknesses. If you have Vericut it's not an issue.

Subsequent ops each then have a new Workpiece under their MCS. It's usually a saved in-process body from the previous op. Keeps things pretty clean.

--
Bill

 

[LMTDCS]

This just seems like a lot of extra work for some simple
machined forms. We have 10-15 of these types of parts a day and run once then never again so every time we add mfg solids it really slows the designers down. We need the cutouts and holes for down stream drilling and wedm (which is a mess right now in nx7 PR Number 6263715, with a priority code of 1 Critical). Is there a way to enforce a cut pattern? By selecting all the openings I get a much cleaner cut but still tries to enter the cutouts. In ideas I could specify the "bridge" length to avoid this. Is this avalible in NX and I am just missing it.

Again thanks.

 

[markrief]

Chris,
I suggest you participate in the nx.cam forum on the Siemens PLM support site. You can reach this from NX using Help --> Online Technical Support --> Electronic Conferencing, or call GTAC and they can get you started.


Mark Rief
Product Manager
Siemens PLM

 

[LMTDCS]

Mark,
Already there.
Thankyou!