Can anyone help me to create this part in Sheetmetal.

[amitshah]

Hi,

I have a cretical part and need to create in sheetmetal.

Is there any way to create such part.

regards

Amit

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[Constantin]

Hi Amit,
this would have to be a welding assembly.
The basic container part can be created using a "Form" feature. The bottom needs to be created separately.

[Dale_Rosema]

Is it a deep drawn part? Would the holes need to be done in a secondary operation?

[TomD.inPDX]

You could make this part easily in sheetmetal using a form or die tool. You will need to model the form/die as a normal part. Please explain why it must be a sheetmetal part? I suspect you cannot flatten it once created as it is a deep drawn part.

This part can be created in several ways. I recommend making it as a part and using the shell command.

To get the cam profile, use the helical sweep function to accurately control the critical surface.

Since you have to make either the male or female side of the die anyway, the sheetmetal creation is secondary process in creating the desired result. To make the die you can begin with solids, or define the surface of the die. See the help files for form tools.

[amitshah]

Hi Guys,

I am more concern about the profile shown(i.e developed view).

I may go for the deep draw operation, but how I can achieve the profile mentioned.

Or is there any other way apart for deep drawing where I can create the mentioned profile.

[TomD.inPDX]

I see, you are asking the engineering question rather than the software tool. No matter what, this is a deep drawn part and will require stamping. Tool makers will make sure you get the part you need in the end. All you have to do is define it correctly. On the drawing you should define minimum material thickness' in highly drawn areas. That critical surface is easy to create by the tool makers.

There is one point of concern on the developed view profile. from 0-90 it is 3.2(Z) then another 3.2(Z) from 90-180, but only 3.1(Z) from 180-270. Did someone get careless or is this the true intent? Does it reach 9.5 just -before- 270? Is there a sharp step at 180 or is it radiused at the step? Technically, this may not be completely defined. Its the little things that can trip you up but as you claim they are critical, these questions should be asked.

You just need to send the complete drawing and probably the 3D model out for quotation and respond to inquiries from suppliers.

If you want a prototype of this part, you may have other options to consider like rapid prototyping or machining.

[amitshah]

From Point A to D the profile gradually varies then it become constant till E, and then there is a sharp step with an angle of 10 degrees.

I am looking for the help to create the model with such profile in Creo/ProE.

[TomD.inPDX]

The drawing reflects a constant rise from 0-180 and from 180-270 it is different... by only a little, but it is different.

You need to use Helical Sweep as mentioned before. Make the model solid and use shell to get the right material thickness. You will model 2 separate sweeps... 1 for the incline and 1 for the decent.

The helical sweep will be a pitch of 12.8 swept for 350 degrees. Trim the face to the 9.5 dimension after the sweep. Now create the sweep in the opposite direction for the 10 degrees down. It will have a very tall pitch of 460.8 for only 10 degrees starting at the end of the previous sweep.

The remainder of the part is a simple revolve and a few offset surfaces for trimming the bottom.

Add appropriate fillet, shell, and add the 3 holes. Done.

Again, the 9.5 dimension will happened just before 270 in what I described. Please review carefully what I have stated before regarding this slope. When someone says "critical", you have to pay attention to all the details. The worst thing someone can do is round input values just to make a drawing. If the real requirement is 9.5 at 270 degrees at a constant pitch, then the 3.2 and 6.4 values are not accurate. Your pitch would be 12-2/3 (12.6666666667) instead of 12.8. See why accurate input is critical?

[TomD.inPDX · Accepted solution]

Sorry for the previously deleted post. I have attached a 3D PDF for how the model is made in accordance with my previous posts (which admittedly has some errors now that I went through the modeling process).

There is some critical data missing from the input drawing. I made some guesses as to what the values should be.

One thing that I ran across, and have run across this before in machine parts, is the filleting of the transitions. These are not mere fillets, but need to be "drawn" from the center. Variable Fillets are not the answer for a true cam following if the contact is linear. You will see what I mean when you build the part.

You can view the attached file with Acrobat Reader. Just click the screen and the 3D will activate.

one thing I learned by doing this exersize is that Helical Sweet -really- needs an Angle option. The value 12.666666667 is always rounded and with the calculation in Creo 2.0 dialogs rounds to the current number of decimals (really poor form, PTC!).

[TomD.inPDX]

If anyone is interested:

Video Link : 3679

[TomD.inPDX]

As mentioned before, radial fillets on linear cam surfaces can be problematic. To insure proper transitions along the rotation, you might consider creating a Wrap feature with the fillets already defined. This image shows the Wrap Section. Relation (circ = 97.5*pi) can control angle control and overall length.

On very important feature I learned with this exercise is that the wrap should have a sketch coordinate system to control the Wrap position. Using the "Center" option uses the center of the sketch for wrapping and the results can be questionable if you have reference geometry past the edges of the sketch. Once the Coordinate system was applied as the wrap orientation, the wrap feature became very reliable.

I have run into this development issue quite often in real life. If you machine linear cams and worry about these types of transitions, please post your reliable methods for controlling radial fillets.

[amitshah]

Hi Antonius,

It was a very great help from you. I tried doing the exercise mentioned by your procedure, but could not able to get the output what is required. If possible, can you help in the first phase of creating the same with Helical sweep.

Thanks

[TomD.inPDX]

Amit, please confirm your software version. Is this the full version or educational?

Do you have more information regarding material thickness and the angle of the cone?

Also the information regarding the CAM follower... is it linear or spherical? What is the allowed radius at the transitions?

Here is what I have learned:

The Wrap method is very accurate except that it will not Shell.

The Wrap method does allow for a swept surface and thickening up to a point.

The Wrap method with thickening will properly control thickness at the rise.

The helical sweep method will shell.

The helical sweep does not create proper transitions at the slope changes for linear cams.

Helical sweep would be better done as a surface with later thickening to control the inner surface radial orientation.

Once I know your software version, I will know how to best help you.