Sketch based sweep pattern on a roll

[Anonymous]

Dear community,

I am trying to make pattern of a sweep on a roll, based on a 3D sketch like this:

However if i mark the points on my 3D sketch in the sketch based pattern menu it creates a pattern like this:

How do I manage that the sweeps are tangential to the surface of the roll like the first sweep?

Thanks for help in advance and best regards,

Lukas

[JDMather]

Expand the pattern dialog box and set Direction 1 and verify Start.

Attach your *.ipt file here if you can’t figure it out.

[Anonymous]

Dear @JDMather,

thank you for your fast reply! If i expand the pattern dialog box, it only shows me this:

If I mark the dialog fields in the expanded window "optimiert->opimized" "indentisch->identical" "anpassen->adjust" (sorry, i have the german version), it doesn't change anything on the pattern.

I also attached a copy of my .ipt file!

Thank you again for your help and best regards

Lukas

[JDMather]

What is it that you are attempting to model - I suspect that there might be a better technique.

[Anonymous]

I am attempting to model a rotor of shredding machine. where seperate parts are going to be welded into the sweeps, that I am trying to build like this:

I have already modelled the part that is going to be inserted into the sweep, which looks like this:

and in the end my final object (with alle the other parts already inserted) should look like this:

So what I am trying to do now is to align the sweeps along the 3D line, as i have posted in my first message and than afterwards repeat that pattern all over the roll. In the end I will try to create a seperate cutting pattern all over the roll which would look like this (I know it looks confusing, but that is the final goal):

Creating that cutting profile is easy with a pattern diretion all over the roll, so the only thing a am struggling with, is the arrangement of the sweeps tangential to the roll surface with a (3D) sketch based pattern, linke in the first post.

Thank you for your help and best regards

Lukas

[Anonymous]

I found a better picture, which shows, what i am attempting to do:

The final solution should look similiar to the picture in the link below:

https://www.google.com/search?q=rotor+shredding+machine&source=lnms&tbm=isch&sa=X&ved=2ahUKEwj6-66Fw...

best regard, lukas

[johnsonshiue]

Hi! The seemingly simple geometry actually is not that easy to create in Inventor. The issue here is the pattern feature commands (Sketch Driven or Rectangular) do not have the ability to "rotate" the target feature along the path. I need to take a closer look and see if there is a better way. On top of my head, I cannot think of an easy solution using pattern features.

Many thanks!

[JDMather]

Looking at those images - I don't think your original Sweep is the correct geometry for the first slot.

Isn't that a simple Extrude?

[SBix26 · Accepted solution]

Here's your file fixed up just a little (2021 file format).  All I did was edit the Pattern feature, and add the Base Point reference (intersection of path and feature) and Face reference (cylindrical face).

---

Sam B
Inventor Pro 2021.2 | Windows 10 Home 2004
LinkedIn

[johnsonshiue]

Hi Sam,

This is a great tip! I forgot about the options. I was thinking this had to be done using Rectangular Pattern (along a path), not using Sketch Driven Pattern. I am marking your answer as the solution.

Many thanks!

[Anonymous]

First of all, thank you all for your support and efforts to help find a solution to the problem! especially @SBix26  for uploading the corrected file!

@JDMather  a simple extrusion is also sufficient, but i tried it with the sweep, as the pattern function was not working and i was searching for other solutions... great YT channel btw!

best regards from germany, lukas

[Anonymous]

Hi everyone! sorry to bother you again.... I finished the rotor and an assyembly (.iam) which looks like this:

What I am trying to do is to make record of the rotor rotating on the cutting profile, which is attached to the rotor down on the right side. therefore I inserted a small shaft into to rotor and attached this shaft to the y-axis (shaft can not be seen in the picture).

Afterwards I connectod the shaft inside the rotor with the rotor via the joint->rotation option as marked in the picture above and shown in the pciture below:

If i press the botton with "automatische wiedergabe" marked with the red ellipse in the picture above it rotates the rotor as I inted to do. If I want to to a record of the movement however it only rotates the shaft inside the rotor. I already tried switching the order in which I marked them for the joint connection but it doesn't change anything. If I grab the rotor "manually" with a left click of the mouse the rotor rotates perfectly fine.

Does anyone of you have a suggestion on how I will get the rotor moving during the recording function?

Again thanks for your help and best regards, Lukas

[Anonymous]

Already solved the problem! I replaced the rotation dependence with an angle dependency between the xy plane and a plane i created on the rotor! now it works perfectly fine!

best regards, Lukas