Inventor Rectangular Pattern Won't Follow Path

[Anonymous]

Hey guys I am interviewing for a company and they mainly make benches and outdoor furniture. I am trying to recreate a few products of theirs but I am struggling with one of them. I have this cut out pattern that I need it to follow along the whole bench. I got the back done and the first part of the curve in the seat, but I can not figure out how to get it onto the next part. Is there a way to get it to just follow a path along all of this or do I need to select a certain plane? I have tried both of those and failed so some help would be greatly appreciated.

This is what I am trying to make.

[IgorMir]

I had a look at your file. Well, there is a lot work needed on it yet. Unconstrained sketches to start with. But I leave it to you to work it out.

Since you are using IV2016 - you won't be able to open the actual file. But here is a Jpeg image as well. I hope - it will give you some of the ideas as to how to handle that model of yours.

Cheers,

Igor.

[johnsonshiue]

Hi Igor,

Yes, I agree. The Sketch1 is not done properly. There are a lot of critical constraints missing. The thickness is not consistent. There will be failures down the road.

The example you provide is excellent! One thing I would do differently is how the pattern is done. I can simply unfold the part into flat shape. Then pattern the feature straight. Then refold it back. There is no need to create two separate patterns.

Many thanks!

[Anonymous]

Well I only got one semester of Inventor in college and the professor did not really do much. So if you could give me a little bit more guidance on how to flatten it and then bend it back I would greatly appreciate it!

[johnsonshiue]

Hi! You can use Igor's part to learn the workflow. The part you attached here does not have uniform thickness due to lack of proper constraints. It cannot be used for sheet metal modeling.

Open Igor's part, move EOP to above the patterns. Then use Unfold command -> pick a planar face -> pick the bend in the middle. You will see the sheet metal part is partially unfolded. Then move EOP one step down to include the rectangular pattern. You can change the number of occurrences so that it will go across the bend. Lastly use Refold command and select the Unfold feature to fold the part back.

Could you try it and see if it works for you?

Many thanks!

[Anonymous]

Yeah I'll give it a try here some time tonight then I'll get back to you. Thanks 

[Anonymous]

 Here is the newest version I believe I did it correctly and it was extremely quick too. It only took about 10 minutes and that was mainly because my PC did not like the Refold command too much. Let me know what you think!

[Curtis_Waguespack]

Hi @Anonymous, 

Welcome to the forum, and nice work.

A few notes:

• When you post a large or complex files on the fourms you can use the End of Part marker (EOP) in the browser, to "zip" the model in order to make the file size smaller, so that it's easier/faster to upload and download.
• Sketch 1 is still not fully constrained, and there appears to be a bunch of "garbage" points in the sketch, indicating that maybe you pasted it in from some other source, such as AutoCAD. All of that should be cleaned up and the sketch should be fully constrained, so that when you click and drag one a line or arc it does not move or distort.
• Sketch 2 is not fully constrained either. Typically we expect performance and long processing times when we see a sketch (like Sketch2 that says 95 dimensions are needed to be fully constrained. )
• When you use the Refold tool you can choose the option to Add All Bends, so that 1 Refold feature is created rather than 3. That is unless 3 were required due to long processing times on your computer as you mentioned. In that case 3 Refolds are fine, if that helps.

Other than that it looked pretty good!

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[johnsonshiue]

Hi! It looks nice. That is exactly what I would do. The only thing I would do differently is that you only need one Unfold and one Refold feature. You don't need to create three Refold features. Here is a trick. You can simply delete the last two Refold features. Edit the remaining Refold feature -> click on Stationary Reference -> pick the Unfold feature -> add all the bends -> Ok.

Many thanks!

[Anonymous]

Okay thanks alot! I am going to completely redo the whole process now and try to make sure everything is done in the proper manner  I will have another post up later.

[IgorMir]

Thanks, Johnson.

Yes I was thinking of Unfold/Refold pass too. But in this instance I just wanted to refresh my memory on Rectangular Pattern tool. 🙂

Cheers,

Igor.

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@johnsonshiue wrote:

Hi Igor,

Yes, I agree. The Sketch1 is not done properly. There are a lot of critical constraints missing. The thickness is not consistent. There will be failures down the road.

The example you provide is excellent! One thing I would do differently is how the pattern is done. I can simply unfold the part into flat shape. Then pattern the feature straight. Then refold it back. There is no need to create two separate patterns.

Many thanks!