Swept Cut that returns path 1

[PieBoy]

Hello all,

When using ProE and i wanted to produce a slot for a spherical ended key, i would sketch a line, and sketch half a ball nose cutter, and ProE would follow the line of the cut and return on the line to produce the round ends.

When I try the same on SW 2007 SP4, the swept cut only produces one side of the path sketch. Is there something I'm missing.

Thanks for any help, cheers Mark.

Tyan Mobo 2xDual Core Opteron 2214
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[josephv]

Hello Mark,

As far as I know, SolidWorks can't do what you describe. You may want to send in an enhancement request.

For now a quicker way to do a slot is to offset a centerline in a sketch and select cap ends that are rounded.

cheers,

 

[PieBoy]

Well thats a pain!!

Can you explain your methods? I have only been using SW for around 6 months, I come from a ProE back ground.

Tyan Mobo 2xDual Core Opteron 2214
4gb Ram
Quadro FX 3500
150gb Raptor Stripe Raid
XP Pro x386 SP2

 

[josephv]

Hello Mark,

It may be a pain now, but many of the enhancements that SolidWorks has did originate from customers like you. So submitting an enhancement request is worth your time in my view.

One way to create a slot is to:

1) Insert a sketch
2) Sketch a centerline
3) Offset the centerline
4) Choose bi-directional, with cap ends, and rounded ends
5) Select the cut extrude feature

hope this helps

 

[PieBoy]

Ah I see, thats a nice feature in sketch, never used that before.

My problem is I dont need a slot for a round ended key, I need a slot for a round key/pin, with spherical ends. So a plane extrude wont produce a form i require.

I could revolve a section on the key, but to make more conplex i require the slots to be joined.

I'm not really procuding a keyway slot, but rather a grease way on a face, produced with a ball nosed cutter. I hoped to sketch the path, giving the CNC operator XY positions, then create the true section showing them the depth based on the cutter they have.

Maybe i should have been more clear.

Tyan Mobo 2xDual Core Opteron 2214
4gb Ram
Quadro FX 3500
150gb Raptor Stripe Raid
XP Pro x386 SP2

 

[Theophilus]

Perhaps you could use a Sweep to perform your cut and then cap the ends with a 90° spherical Revolve? The Sweep, at least, will follow a path through turns instead of only a single line segment (not sure if you need that).

Also, SW 2008 is supposed to support a limited degree of swept solid forms (like a ball end mill). I'm not quite sure of your specific application, but that may also work. (I'm also running SW 2007, so am not sure of the limits of this newer feature.)

Josephv, thanks for the nice explanation of the offset, capped slot tool! I can hardly believe I've overlooked that in the past, it's so useful (star).



Jeff Mowry

http://www.industrialdesignhaus.com

A people who value security over freedom will soon find they have neither.

 

[SincoTC]

To cheat a little, provided you need a round bottomed slot that's equal to or more than half its width (radius); create your slot as per josephv's method (with square capped ends if you like) and then apply a fillet to the long edges that is one micron or a tenth of a thou less than the radius, so that in theory there is something left of the original face to fillet to, then you should get what you want without much fuss. In most instances, the minute flat at the bottom centreline and the top edges won't matter.

Trevor Clarke. (R & D) Scientific Instruments.Somerset. UK

SW2007x64 SP3.0 Pentium P4 3.6Ghz, 4Gb Ram ATI FireGL V7100 Driver: 8.323.0.0
SW2007x32 SP4.0 Pentium P4 3.6Ghz, 2Gb Ram NVIDIA Quadro FX 500 Driver: 6.14.10.7756

 

[Theophilus]

Or use the Full Radius option (might have to revolve the ends to get the spherical feature after the Full Radius).



Jeff Mowry

http://www.industrialdesignhaus.com

A people who value security over freedom will soon find they have neither.

 

[CorBlimeyLimey]

You could sweep-cut a semi-circle along a flat bottomed 'u' shape path. See attached.

 

[josephv]

sorry, Mark, I obviously misunderstood your question.

all good ideas, another approach

sketch a semi-circle and make an extruded cut
do a revolved cut of the semi-circle on both ends