Solid sweep cutout

[ota_poul2]

Hi Edgers,

I need a little bit help with Sweep Body Cutout command.

There is a known limitation with this command, when you want to use for example circle sketch wrapped to cylindrical face as trajectory.
The task is to cutout a groove or slot with the help of tool body which is guided along the wrapped sketch where the tool axis is continuously changed and positioned perpendicular to the selected cylindrical surface.

Curently I am looking for the simplest workaroud for this. I am able to WA this using quite complex surfacing and 3D curves modeling, but maybe I am missing a simpler WA.

I attached a short video and simple part for better understanding.

Ota

PS: @Imics, I am betting all I have on you :-)

[Imics · Accepted solution]

Hi my Friend,

I have a bad news for you, there is no way to do what you want with SSC. There are two issues one of them is the wrapped sketch other is self-intersecting result... 

There is an other way, but the surface will be rough and the last is simulating in a CAM software. My colleague was so kindly and programmed this part in Edgecam and saved it as stl.

BR,

[RyanM]

So, this isn't the same code as was used in NX? NX allows for the self-intersecting. That's strange that Siemens would put that limitation onto this function. Kinda defeats the whole purpose of the function. Don't you think?

[ota_poul2]

Hi @Imics

thank you very much for great video and for the attached part - you are not only "SE Phenom", but you are "SE GOD" :-).

I knew there is a some way with using pattern along curve feature, but I was not able to get a final feature.

Well, this issue is now logged and exists as ER8901823, so anyone can join.

@RyanM: I also think this is different code from NX.

Ota

[Imics]

@RyanM, @ota_poul2 I've tested it in NX11 and it couldn't solve this challenge... There are some cases what I could solve in Solid Edge but couldn't in NX with SSC... So I cannot say, that SSC implementation is weakest in SE compare to NX, nor yet...

BR,

[paul_busengdal]

Good Day ota_poul2,

In your sketch used for wrap sketch I would create an offset equal to radie of tool in both directions of the curve. Close the ends of the sketch and do a new wrap sketch with the new offset curves. Finaly create a normal cutout to the depth required. This should give the same geometry if the end of the tool is flat. If the end of the tool has a chamfer or rounded, create a chamfer or round feature on bottom surface in groove

Best Regards

Paul_Busengdal