How Can create a Sweep with normal to projection as centre axis

[ruk]

I want to create a groove on a cylinder as shown in the image. I create the groove path and wrapped on the cylinder

I am using sweep to create the groove, if i select normal to trajectory the sweep cut is created on cylinder. but for manufacturing i want to create the cut normal to center axis.

if i choose normal to projection and select ctr axis sweep feature failing. It will be helpful if anybody can suggest a solution.

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[ruk]

Hi Steven,

Pls find the below image of cross-section

[dgschaefer]

Can you clarify what you mean my having the section normal to the center axis?

Having the section plane always normal to the axis would make it always paralel to the ends of the cylinder, so there would be no cut at all on the horizontal parts of the path (assume the cylinder is set upright). Keeping the section plane always through the center axis would produce no cut in the vertical parts of the trajectory.

I'm not sure what you are after. Perhaps an understanding of how it will be manufactured will help.

[ruk]

Hi Doug,

please find the below sweeps

Pink Colour-Section plane normal to projection and i selected ctr axis of cylinder.

Green- section plane normal to trajectory.

I can use this option for simple curve, if the curve is bending i am not able to use normal to projction by using ctr axis.

I am planning to machine this grove using 3-axis machine, if the section is normal to trajectory 5-axis machine needed to manufacture this part.

[dgschaefer]

The "normal to projection" is not easy to understand when picking an axis. Typically a plane is selected and the section plane is kept normal to the trajectory as if it were projected on that plane.

That idea doesn't really apply if using an axis, however what it appears to do is keep the section plane through the axis. With your trajectory, that isn't going to work as you have vertical section in your trajectory where the section would become completely overlapping.

Put simply, this is a geometry problem, not a Creo problem. You can try creating it in multiple, shorter sections, and create the parts that go vertical separately in a different way.

Another way to accomplish this kind of sweep is to select the circular end of the cylinder as a second trajectory and use it as the normal trajectory. I think you are still going to have trouble with the vertical parts, however.

[JonathanHodgson]

Looking at what you're trying to achieve (and how you plan to mill it - and I think you want to use a 4-axis machine?) I would suggest a different approach.

1. Extend the profile to become a surface, to the required groove depth
2. Thicken the surface to produce a cut
3. Apply a full round to the base of the cut

I'm not sure of the best way to achieve 1), but hopefully others may offer suggestions on that...

[TomD.inPDX]

This type of feature for mere CAD work is fairly simple and it will do what you expect by default and you have to create a revolve cut at both ends to complete the feature. You do want -normal to trajectory-.

I use to make tubes with worm-cuts like that in CAD with a little more complex cutter shape. The problem comes in when it turns corners. The fact that the cut is a planer profile rather than a 3D cutter profile make the shape slightly different in certain cases.

The operation is straight forward... you use a U-shaped cutter on a mill and rotate the cylinder as you move the cylinder laterally. That cut -is- a 3D cut, not 2D. You can create the sweep as shown above, but when you create the revolve cuts at the end, try patterning it tightly along the trajectory and see if there are not some new cuts being created. You might run into some issues with this (error features) but it will give you an idea if you fall into that special case. You might need to play with the accuracy settings for better results. These features will create very small cuts where most will be line-to-line.

[TomD.inPDX]

I have attached a sample of what I am referring to. Activate cross section A and look in the inside radii of the cut. You will see a sharp transition at the quilt (surface sweep) and the patterned revolve cut has a curved transition trend. This is very much radius dependent as the process creates a pinch point as the radius of the cylinder is reduced. This pinch point needs to be accounted for in the wrap if you intend to have a radius at each bend -into- the part, not just at the surface.

Again, if the radii are sufficient in the sweep trajectory to the depth of the cut, your model will be correct. But if you are allowing -reversing- with the tool, the model -will have- a slight inaccuracy. The mill doesn't care, but Creo simply doesn't do cuts the same way a mill does.

The attached file is Creo 2.0. There are some useful tips in the models for creating referenced patterns along a 3D curve profile.

For you Creo Manufacturing Extension people... If you machine this, does it emulate a rotary cutter correctly or does it also sweep a 2D profile?