linear pattern not working on sheetmetal parts?

stvnvl_8501

I need to copy a certain feature a bunch of times in a sheet metal part (and preferably even to other sheet metal parts , in same part studio) . 
but I need to finish the part before anty type of pattern/ paste of features will work? problem is: features added after finishing sheet metal part are not showing up in the flat pattern...
some examples in this particular example: several tabs to connect 2 sheetmetal parts, (see picture)  to be placed at specific locations and merged with existing geometry. 
it's very tedious and error -prone to design (and later maybe update) evey instance by hand... rather use 1 master feature to copy and keep associativity to this one "master". (one can imagine making a library of regularyuse sheet metal features to re-use throughout)  I tried a whole lot of different approaches: tried designing it in a separate part studio as 2 seperate part, one body  to subtract and one body to add.  and then deriving it into the sheet metal part studio, adding it to the parts with booleans. again no luck with sheet metal, only with "finished" sheet metal or solid parts.  
what would be the way to go about  copying certain features at specific places in a part studio? 

other example is a  venting louver to the side of the part that uses the same sheet metal feature and that is then only a simple rectangular or circular pattern.

David_YL_Nguyen

Hey @stvnvl_8501,

Could you share a link to your (public) document so we can have a closer look?
I tried playing around with some linear patterns in sheet metal parts and worked fine for me. Maybe you try to do something more complex.
Would be interesting to take a look. Thanks

https://cad.onshape.com/documents/6ca37af9d7b3a8765d2c28ac/v/6886669a2c0155a28211c72d/e/91603e881b20689ebc569158

stvnvl_8501

hi @David_YL_Nguyen
thanks for the swift reply. I'll prepare a sample tomorrow as I can't share the actual design I'm working on. Or I'll do so in your shared file. 

stvnvl_8501

I'll have to rephrase, face pattern is not working in sheet metal. so you would need to copy the extrude feature (the hole) seperate from the flanges in a similar/ the same array. 
How would you go about getting the same feature in the next sheet metal part? I've tought about having some sort of basic sketches in a seperate partstudio and deriving these to re-make the same (series of) features on seperate parts (or different faces of the same part for that matter) thus being able to control them from a central place... 
 

bryan_lagrange

Here is a link of similar pattern in sheet metal. Hope it helps.

https://cad.onshape.com/documents/687fd891217da43ad2cc4a2f/w/bb014e50b261960d5940aa8e/e/539c200e10cdb989e3289396

stvnvl_8501

thanks @bryan_lagrange interesting approach. It sparked an idea. Ill report back tomorrow. 

mfalkensteiner

Hi @stvnvl_8501
If you want to reuse recurring shapes or bends as templates, I recommend the Sheet Metal Forming Tools feature:
https://cad.onshape.com/documents/a752e0db24eb071ebb6f5aa0/w/47c6a6888718e30c80f1f652/e/e5c2abf7dd42d71d28468eca

eric_pesty

mfalkensteiner said:

Hi @stvnvl_8501
If you want to reuse recurring shapes or bends as templates, I recommend the Sheet Metal Forming Tools feature:
https://cad.onshape.com/documents/a752e0db24eb071ebb6f5aa0/w/47c6a6888718e30c80f1f652/e/e5c2abf7dd42d71d28468eca

That's not quite the same as anything created this way won't be in the flat pattern.

David_YL_Nguyen

Hey @stvnvl_8501,

Here is another approach for it. I have looked at two options that could help you out:

1. Using the Fold SM Featurescript: You can use this FS in conjunction with a sketch. You can use the same sketch and fully define it and then copy and paste from/to different planes/parts/etc. I was struggling every now and then as it seems this FS is a bit particular with the definition of the fixed edge or face.
2. Using the Point Pattern FS: Limitation here is that it seems to be only working on the same plane and orientation.

Link to my document: https://cad.onshape.com/documents/6ca37af9d7b3a8765d2c28ac/v/6f5fdb72ab2044e372749ef9/e/fce0ae8033af329258f47c49

Hope this helps. Curious to know how you are getting along. Cheers

stvnvl_8501

Hi guys. 

Thanks for the help! , been at some other stuff last couple of days. will look into it today. I'll keep you posted. 

stvnvl_8501

Hi,
 I can't get it to work like I'd want it to. I made the "feature" in a separate part studio,  dimensioned to fit the 2 parts in the part studio I need to copy it to. same gap etc. added another volume as a cut tool for a boolean. 
apparently add boolean between 2 sheet metal parts isn't working well. judging on @bryan_lagrange 's post I thought It would, but it doesnt. I hope I am missing something here... @David_YL_Nguyen I was using the Fold SM Featurescript as well. and indeed I have no idea were or how It decides to place the fold line relative to the final position of the folded plane or how to influence this. 
please take a look. 
https://cad.onshape.com/documents/79aa8cf485b7b4c243ed3fc3/w/363901e34f7de9cad4bfaa30/e/69db83902539beaa2ec80ba0?renderMode=0&rightPanel=sheetMetalPanel&uiState=6523f34ecf7b4157262af59f

David_YL_Nguyen

Hey @stvnvl_8501,

Yeah unfortunately boolean between multiple sheet parts does not exist for now. I think the initial example was just a pattern of one single part.

Please check again my "Fold SM Test" tab in my document. I would suggest you use this with a sketch just on a flat area and then apply the Fold FS.
I cannot check how you are using the feature as you are only link sharing. Cannot go through your feature tree or copy your document.

Let me know. Cheers

stvnvl_8501

Hi @David_YL_Nguyen
How do I share it the correct way then? 
what I need is a correct/ specific distance between the underside of the tab and the top of the sheet folding out the tab from a U-shaped cut in the sheet.
pretty common I guess? 

eric_pesty

@stvnvl_8501
One way to do  this is to do two 90deg flanges and then use a move face with the rotate option to get the angle

David_YL_Nguyen

Hi @stvnvl_8501,

If you make your document public with permission to copy, we can have a closer look.




If you design your flange using the bend features you should be able to measure the correct distances for your bendlines to then be able to use a sketch together with Fold FS.

stvnvl_8501

Hi @David_YL_Nguyen
I have the document now set to public. 
test_sheetmetal_features_copy (onshape.com) 
I haven't found a similar way of controling the position of the bend as you have with the "SM flange" feature, where you have tehe option to choose outer/ inner/ holf line etc. seems rather arbitrary. I can move atherwards to the right position but then the flat pattern is conflicting of the gap becomes uneven. The thing I need I to "fold out" the tab to a specific distance. it's important to get this right because it's the base for a specific stamping tool.

David_YL_Nguyen

Hey @stvnvl_8501,

This is not currently possible:

I haven't found a similar way of controling the position of the bend as you have with the "SM flange" feature, where you have tehe option to choose outer/ inner/ holf line etc. seems rather arbitrary.

Please have a look at my document Tab "Fold SM Test 2".

I know this is only a workaround but this is what I would do:

1. precisely create one flange with the distances I need
2. copy the dimensions from the flat pattern including the bend lines
3. Create a new sketch (fully defined) to use for a cutout
4. Place that sketch (copy + paste) wherever needed 
5. Cutout (Extrude/Remove)
6. Fold FS

Hope this works for you. Otherwise, I feel like I still have not understood what you need to do.

Let me know. Cheers

bryan_lagrange

Here is a method to use linear pattern.

https://cad.onshape.com/documents/068f35af42a4b73acc86ded6/w/dabcf5a789ed29622585dc2c/e/23f206ecc7dd045e4f05e33c

glen_dewsbury

Another option that takes a fair bit of setup if you think it's worth it. I did this out of curiosity and as a challenge.
Advantage is that it can be done with random patterns as well as linear.
The tabs in part one looked the most straight forward until I tried to offset at an angle.
Had to play around a bit to find blind lengths for each leg in part 3. Did not work when selecting sketch entities for tab lengths and angle geometry. All the tabs came to the same entity so only the seed was correct.
This is also set up for max tang length using  .005 laser cut profile. There is a slight error at the flat cut out. I'll leave that for you. LOL
Learned something new today! Wasn't aware random faces could be selected all at once to make flanges.
https://cad.onshape.com/documents/e3d38259440626b10783e1c1/w/6822d97fb9a4582249feb1c4/e/bf619fc2c901a34d102cf926

stvnvl_8501

thanks guys, all great approaches to the challenge. Found a workaround myself as well. ! drew the tabs / hooks/ clips in a side view to the precide dimensions I need.  (much like you  did.) and converted this sketch to sheetmetal. then proceeded sketching on the flat pattern to get the surrounding geometry to join closely with the geometry of the tab folded flat. sheetmetal tabs | hook_feature (onshape.com). I now can use point derive to add this feature to (finished) sheet metal parts. I hope the sheet metal worker will figure out how to get it to a flat pattern... ;-)