Every time I convert a part to sheet metal the auto relief messes up my part, How do I shut this off?
Set up a new template file where the setting is off by default. You will need to create a simple sheet metal part with the appropriate settings, then delete all the features before saving off your template.
But How do I open an existing part in a template? these are existing parts not done in solidworks.
Paul Clor wrote: But How do I open an existing part in a template? these are existing parts not done in solidworks.
Paul Clor wrote:
This post explains how to open an old part with a new template.
how to change part template for an existing part
This did not work I made a template turned it off brought the part in and it still adds the auto relief. Any thing else I can try? I mean I can redraw the parts as sheet metal but doesn't that defeat the purpose of having convert to sheet metal.
the template does not hold it turned off... Can Anyone help with this?
I don't think you can get away with it, I would just add material there if you don't want the relief cuts.. Frank Ruepp might be able to explain why it does this and if there is a way to turn it off completely..
So I made the template turned it off, brought the part into the template and that fixed nothing at all.
After googling what to do I see lots of past forum discussions about this and I see no answers everyone pretty much says it can not be done. So I guess this is not a time saving tool and just redraw the parts is the answer. Really wish this would just work.
The Auto-relief is part of the bugs SolidWorks has to fix because it can't be turned off as far as I'm aware.
You can use different auto-reliefs which sometimes help to get the result but I usually just try do and do my design otherwise. Make it longer and cut what I don't need, add material, whatever works best in the particular case.
When I read your originial post (Every time I convert a part to sheet metal...) and look at the screenshot you provided I suppose that you are using the Convert to Sheet Metal feature. Even though you have turned off the Auto Relief option in the feature:
You still can get some sort of relief since the algorithm analyzes the geometry and determines that a relief is required in order to be able to flatten the geometry at all. And since the primary goal is to get a sheet metal body rather than failing the conversion we add "necessary" reliefs.
So when you use the Convert to Sheet Metal feature you might have to add material in the flat pattern and "clean up the mess". Since the material will be added after the flat pattern it will not be propagated back to the folded state and will only be visible in the flat pattern.
Another solution could be to use "Insert Bends" rather than using Convert to Sheet Metal:
Insert Bends is a completely different feature that uses a different algorithm which might be in some cases be a better choice. I created something similar like your example and it actually did not create the undesired reliefs. But as I said: "Something similar" and not exactly like yours so no guarantee that it works for you as well:
At least in my example it created kind of smooth corner after I had turned off "Simplify Bends":
But on the left hand side it created kind of a visible dent which might be related to my sloppy modelling technique. But I just wanted to whip something up in order to have a similar case...
...and to finish up my post with a personal note:
Back in the days when I was doing SOLIDWORKS demos I was quite often confronted with imported (sheet metal) geometry from other CAD systems and I was supposed to create SOLIDWORKS sheet metal parts from those. The first priority has always been to be able to flatten the part! Since different CAD systems have different defintions how a sheet metal part is defined I had to sometimes remove geometry that prevented me from unfolding the part and add this geometry again after the flat pattern. So don't expect a "perfect" sheet metal part in a "one feature operation". If it works this way: great! If it doesn't, you will likely have to manually fix issues...
Hope this helps.
SOLIDWORKS Product Definition Team
Does it matter I am using 2015? I can redraw the parts as sheet metal that is not a problem it's only when I try to convert a part that is originally a step file.
no it does not matter that you are using 2015. The behavior is identical. As I explained in my previous post the process of creating, respectively converting are different animals.
If possible I would try to convert the existing imported geometry rather than creating it new from scratch even if it emplies some extra work to "prepare" the geometry to become a sheet metal part. Sounds like a lot of effort and in the worst case it is even error prone.
SOLIDWORKS Product Defintion Team
If I may add to this, I sometimes need to modify the function within the body and not within the feature tree in order to get the result I want. It has nothing to do with sheet metal conversion but thought I'd just pitch this out there.
This is where I mean:
Yeah I do that too
I tried everything everyone has suggested and this what my parts look like after converting them
Have you tried "Insert Bends" as I proposed in my earlier response?
I suspect from his earlier posts, he is importing an already formed part and then attempting to convert and flatten the part. Will insert bends work for this situation? If so that would be great but I have never attempted it and would expect it not to.
I personally don't like to convert and prefer to remodel as much as possible. Then I can have the features how I want them even if it takes more time.
Paul, I think the "work around" that has been mentioned is what I would do in this case. If you import the part and it comes in with the relief cuts you can accept it that way and then go to the flat pattern and add the extrusions to clean things up. This was you can get the plasma cut that is desired but the part will still form. Doesn't look quite right in the formed version but it will get the job done.
Insert Bends was the first sheet metal feature ever in SOLIDWORKS and it can handle imported geometry as long as there are some requirements met:
If you follow those guidelines you should be fine to use the Insert Bend feature.
And Jim Steinmeyer, I totally agree with this:
<<If you import the part and it comes in with the relief cuts you can accept it that way and then go to the flat pattern and add the extrusions to clean things up. This was you can get the plasma cut that is desired but the part will still form. Doesn't look quite right in the formed version but it will get the job done.>>
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