SMT extruded cut normal to surface

[BartL]

Hi All,

I'm using Creo 8.0.

Hopefully somebody here can help me out since I haven't been able to find a solution on the internet yet.

Quite often I have to design tubes which will be cut from sheetmetal and then rolled into their round shape. Therfor all cuts need to be normal to the sheetmetal plate. So far so good. However when I need to make a simple angular cut at the end of the tube things get frustrating pretty soon.

When you look at attached cross section you will see the upper end is exceeding the cutting line. Here I've used normal to driving surface. When I use normal to offset surface the upper end is fine but the lower end is exceeding. I do understand what it is doing so this still makes sense to me. Therefor I would expect "normal to both surfaces" should do the trick but this feature doesn't work at all. 

This is frustrating cause a simple cut like this can't be done in one feature but always requires more features.

Am I missing something here or is it just a bug?

[tbraxton]

One way to do this is to unbend the cylinder and create the cut on the flat part. Are these cuts made to the flat pattern blank before rolling the tubes when fabricated?

[BartL]

I know, but the formed part creation is the goal. So working from a flat blank is not preffered. Besides this, usually these cuts result in very complex flat state contours.

[MartinHanak]

Hi,

edit definition of the cut and click  button. When clicking the button you are switching between sheetmetal cut and solid cut.

[BartL]

This is the feature I was talking about. So yes I'm using this feature but it's not working properly.

[MartinHanak]

---

@BartL wrote:

This is the feature I was talking about. So yes I'm using this feature but it's not working properly.

---

Hi,

in Creo 8.0.4.0 it is working properly. See attached file.

[BartL]

Please read the question. In your example you're not cutting normal to the surface. I need to cut normal, however I need to avoid this exceeding volumes at either the upper side of the lower side.

[kdirth]

I believe you are looking for this:

The circled setting is the key to preventing exceeding the cut line.

[BartL]

I know this function. I wrote the following in my first post: "Therefor I would expect "normal to both surfaces" should do the trick but this feature doesn't work at all." 

BUT I just found out it is working when I let my sketch exceeds the boundary of the part. So it fails when I use the references like you used (which is most common) but it works when the sketch gets a bit of an offset. Strange...

[MartinHanak]

---

@BartL wrote:

Please read the question. In your example you're not cutting normal to the surface. I need to cut normal, however I need to avoid this exceeding volumes at either the upper side of the lower side.

---

Hi,

I am sorry, the 1st version of prt0003 is really my fault.

Now I am sending 2nd version of prt0003. I am sending it to show that the geometry is correct. Display x-section and modify angle of DTM1 plane. You will see that in every situation xsection edge is perpendicular to sheetmetal surface.

[BartL]

Yes, but again... this was not the question.

If you look at your front surface and select the sketch of your extruded cut you can see the material of the lower side is exceeding you sketched line. Now go to edit definition and try to select "normal to both surfaces" you will see it doesn't work.

[MartinHanak]

---

@BartL wrote:

Yes, but again... this was not the question.

If you look at your front surface and select the sketch of your extruded cut you can see the material of the lower side is exceeding you sketched line. Now go to edit definition and try to select "normal to both surfaces" you will see it doesn't work.

---

Hi,

my last reply ...

normal to both surfaces in my model failed because of 360 degree rotational geometry. I removed 1/2 of the pipe and Creo regenerated failed feature successfully. Later I realized that I can use 271 degree rotational geometry. For 272 degree rotational geometry normal to both surfaces in my model failed.

[BartL]

Exactly. However I need a 360degree (or almost) to get a tube. So exept for my just discovered workaround (sketch larger than the tube diameter) it's just nog working. Should be solved by PTC imho.

[StephenW]

I would suggest you should file a tech support case. It's odd. I thought it worked for me but after a regen, it was gone and i couldn't get it back.

I was limited at 270 degrees also

**edit** I did get it to regen once I extended my cut out farther as you said

[BartL]

In your case it worked befor a regen, that's not the case by me. As soon as I set the extruded cut to "normal to both surfaces" it shows directly it's not going to work.

Extending the cut seems to be the best work around for me. Maybe I will raise a ticket at tech support to at least file this issue. Can't imagine I'm the only one struggling with it.

[kdirth]

After a bit of testing in 7.0, I have may have found the problem.  If I make a cylinder and convert it to sheetmetal then make the cut, drawing from silhouette to silhouette, the cut fails.  If I create a sketched rip to break the solid cylinder first, the cut works just fine.  Creo seems to have trouble making the both sides cut when the model is not developable (no rip in the cylinder).