Changing orientation of flat pattern

[Nikola_Perunmoto]

Hi folks. 

I designed sheet metal component (motorcycle luggage rack). Picture below. 

Model orientation is Z up, here is the picture of top view with X axis marked.

And I created flat pattern. Picture below, with added X axis and blue line. 

Is there a way to change orientation of flat pattern? As shown on the upper picture, it is positioned weird related to X axis. I would like to rotate it so "blue line" is parallel to X axis.

I would like to do that because we are machining our parts and making CAM setup will be much easier if I could change orientation of flat pattern.

Any ideas?

[SwApNiLbAd]

Hi @nikolaC9QXB to change the orientation you should use the copy/move command (just type M) to change the orientation of your pattern in cam i think copy/move command will not work so use it in model then go to cam.

i hope this will help you if yes then make it a solution for your question.

thank you.

[etfrench]

Rotating the model in the model workspace is a wasted step when using CAM to create the finished product.  Simply set the Z and X directions in the CAM setup dialog.

[Nikola_Perunmoto]

Hi @SwApNiLbAd, thank you for your time and effort. 

Model orientation is correct. But when I make create flat pattern out of it, it is oriented "strange" - outer edge of angled flange edge is parallel to X axis. 

Here is the model top view. 

And here is flat pattern top view. 

Unfortunately, I can't use Move/Copy command on flat pattern.

[etfrench]

You can also set the Home view:

[chrisplyler]

Which of the three primary faces did you click on (to designate the stationary face) during the Flat Pattern creation process?

[Nikola_Perunmoto]

Hi @chrisplyler, thank you too for your time and effort.

XY face, that is top surface of the model shown (Z up is my default setting). 

But no matter what face I select (top face, bottom face, face of the one of the flanges) while creating Flat pattern, I always get same flat pattern (oriented the same). See the video, please. 

[chrisplyler]

I understand. I think that's weird. I don't know why it's a problem though.

You can orient it however you want in the CAM environment, or if you're just outputting a DXF to use on a laser cutter or a waterjet, you would presumably orient the DXF however you want within the layout software of that machine.

[gottbrath]

I have this same problem! its problematic because the machine software I am using (fabcreator for fablight laser) does not yet have the ability to rotate the dxf in their software. They say its coming, but no help right now

[etfrench]

What problem are you having? Creating the CAM toolpaths or exporting with a specific face oriented to the XY face?

[FormStudio]

I am having the same issue. The flat pattern orientation is not the same as the folded model.

When you then create a drawing from the flat pattern it maintains the wrong orientation. This causes an issue with dimensioning and annotation for fabricators.

Any suggestions on how to resolve would be appreciated.

Cheers.

[HughesTooling]

@FormStudio  You can rotate the flat pattern in the 2d drawing workspace. The challenge is figuring out the angle, you could measure in the model workspace may be?

Mark

[HughesTooling]

@FormStudio  Here's a workaround using Look At then creating a named view in the flat pattern. The view is created edge on but you can then create correctly aligned projected views from the base view.

Mark

[TheCADWhisperer]

---

@Nikola_Perunmoto wrote:

I would like to do that because we are machining our parts and making CAM setup will be much easier if I could change orientation of flat pattern.

Any ideas?

---

For whatever the information is worth - here is how it is done in Autodesk Inventor Professional...

Students can download Inventor Professional for free from http://autodesk.com/eduction

[video]

[FormStudio]

@HughesTooling  This is awesome.. that worked exactly as I needed.

Thanks so much for your advice it is very much appreciated.

Thanks to @TheCADWhisperer  for your replies as well - appreciate the intel.

Cheers. 👍

[Anonymous]

Just find the angle between the layer below blue line with x-axis and rotate the enter body with that angle by specifying the angle of rotation through and a specified layer i.e., the layer below blue line taking the axis of rotation as the axis perpendicular to the design

[etfrench]

Relying on the Measure tool to determine angles to move is not the best practice.  The Measure tool rounds the value so it will only be as accurate as the number of decimal places displayed.  Use joints for precision.

[Anonymous]

May be we can project the edge and take the measure option right.

I know that will be bit extra process. 
It can be one of the options. Isn't it?

[HughesTooling]

@Anonymous  I pointed out in post 12 you can rotate the view but there are 2 problems, one as @etfrench  points out the angle could be to many decimal places and 2 it's not parametric so changes to the design will change the angle. The use of a named view as I show in port 13 should be more reliable. There could still be a problem if the part is rotated in the model workspace because you can't accurately edit a named view.

This is a problem for the 2d workspace in general, if you rotate components after creating a drawing, even if you have named views you can't realign the 2d drawing without creating new named views. I've asked support about this quite a few times and never got any answers. What's really needed is an associative named view similar to a joint origin so the view moves with the component.

Mark

[Anonymous]

I encountered similar problem, think I solved it in this way. 
Before drawing go to Preferences -> Default Modeling Orientation -> select Z up.  

My problem was every time I unfolded it produced a pattern that faced 'Front' view as top. If you set Z up at the beginning of your drawing that should help align things. 

This might not be the solution for you. Just noting here for those who encounter my version of this problem.