I have a sheet metal part with both countersink holes and embosses, how do I keep these when I convert to sheet metal and flatten the part?
If I understand it correctly.
You can create a configuration if you don't want to see it on a solid model.
You can hide the elements you want on the driwing page.
In DWG you can delete the elements you want.
What I want is actually to keep the emboss on the sheet metal part - also in the flatten state.
At the moment there is no straightening feature for SW forming tools.
Maybe in future versions.
You need to use Configuration.
I don't need a straightening feature, I just want to keep the emboss in the flatten state.
I think is possible....but I need to start from a scratch
If you convert it to sheet metal doesn't it able...
Add a configuration and model what you want to see after the Base Flange, use the original configuration to show your flat...
Is that what you're talking about?
see you attached video.
If I understand correctly, you have modelled the part and are then using the Convert To Sheet metal feature which requires you to select a fixed face and bends etc.
If this is the case then I suggest using the Insert Bends feature instead. I have used your enclosed file. Choose the narrow fixed face and add your bend radius.
If you do want to hide say the Countersunk feature from the flattened view then edit the Flat-Pattern feature in the feature tree, Select the Faces to Exclude box and select the countersunk faces.
Hope that helps.
This is what I was looking for - Thank you :-)
... but can you tell me why it won't work on this part?
Victor Fagerlund wrote: Hi, I have a sheet metal part with both countersink holes and embosses, how do I keep these when I convert to sheet metal and flatten the part?
Victor Fagerlund wrote:
When you flatten a sheet metal part, you're showing the flat sheet stock, outlined to the required blank.
So the csink through holes would be shown (as Mr. Loftus showed above) but not the emboss as dented.
If you need to display an interim fabrication step, I'd create a configuration to show the emboss.
This way, the flat pattern is left as is and you have the starting flat state, then the dented state and the formed state each available.
Another suggestion is to create this part from the start as sheet metal using the Base Flange command.
I don't know how you created your emboss, but for sheet metal, you use form tools to make such dents (and others).
The form tool can be shown on the flat in one of 3 states: formed, outline or center point.
This is set in Doc Properties>Sheet Metal. But it's set for the document, so if multiple stages need to be shown, then Blather I configs are still required.
Examining these images taken from above, I don't believe your emboss will be formed close to what's shown.
The inner edge on the left (red line) has no radius which is a sheet metal no-no.
I can't tell from your image on the right if it's the same situation, but I suspect it is.
This is another beneift of using the form tool.
SW doesn't allow your to create a form that would either violate material flow (as this is a lossless operation) or violate tangency at all transitions (another sheet metal no-no).
To complete the form, the form tool must be modelled properly else you'll get an oddly worded message roughly stating the above paragraph.
So you must return to your model and make edits, which usually means larger radii and the subsequent edits due to this. (Generally r=2t min on the stop face side.)
From what I can gather from the images, I don't believe your modelled emboss will be close to the actual one as the modelled emboss looks more machined than formed.
I hope this helps.
Keep in mind that I have NOT designed the parts. I'm not a designer, I'm a toolmaker - and the only thing I get to work with is a .stp file.
What I want is a couple of configurations to show the different states of the parts according to the actual production.
I need the parts in different states with the emboss and countersinks so I can model the tool.
Mike showed me an approach I didn't knew on how to flatten the first part. It works great on the first part, but it troubles me on the second part I have attached.
If someone can help me with this - please let me know :-)
I made it but you must to fix the product
But if you move 0.25 that faces it will be works
This looks interesting! - can you upload the part? :-)
Yes I did it...made on SW2018SP3
Ahh... I'm only on 2017 :-/
Can you please explain what you did?
It is hard for me to tell just from the pictures :-(
When I go to the office I send you each step on a separate XT file to you.
Added....I will made a video for you try to see step by step each instance....
In this second case the issue is down to the model geometry as Ruben Balderrama says.
This is hard to spot in the original step file but when you flatten the model 2 of the tabs merge with the rest of the body and so fail.
To show this i have made a 0.5mm cut on both tabs before using insert bends. You would have to do this in a more accurate way to suit the design.
Sometimes when receiving a model as a dumb solid or in this case step file, you may have to make adjustments. Move Face, Move/Copy body are good for this as are some of the surfacing tools along with the usual SW features.
I hope this shows in the enclosed images.
That was I fix it, but I use move faces...
This is actaully not the case, I have no issue with the two small bends.
Maybe I use another bend allowance.
My issue (I assume) is with the bend as shown in the below picture:
I think a process by punching on this component won't be able to make it.
Maybe like this to make it and at the same time maybe will cut it by Slitting
Hey Victor Fagerlund how you made the process for this blank?
To make it able by punching you need more space (see a layout by punching) as obvious reason a punch wont be least than 5mm
We laser cut this part, and afterwards use a tool for the bends.
Excellent choice! Show Us a final product!
I will :-)
But I still can't figure out why you don't get the same errors that I do? :-S
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