After years of using sheet metal, my first try in weldments.
What's this extension and how can I prevent it.
Because of this, cut list's length shows as 262.34 while it should be 234.0
Assembly and used structural Member is attached.
Any kind of advice is appreciated.
Hi Habib,
You need to use the trim/extend tool in SolidWorks:
Have a play around with it to see how it behaves.
Hope this helps!
F
Fernando Castellanos wrote:
Hi Habib,
You need to use the trim/extend tool in SolidWorks:
Have a play around with it to see how it behaves.
Hope this helps!
F
Hi Fernando,
Sorry for not mentioning. I'd already test that one.
It gives me the following error.
Bodies do not trim each other completely. Please Check your input.
thanks.
Ok, so this editor is stupid and I cannot upload videos (for some reason...)
First, you need to create a reference plane on the edge of your profile:
Then, go to your trim/extend tool and input your bodies (change the trimming boundary to Face/Plane)
Discard the part you don't want to keep.
Should work
Fernando,,, I thought that would work also with the Trim/Extend command but it would not let me select the planes for the trimming boundary. Also tried a planar surface to no avail.. Thought I was able to do that in earlier versions.. I have no memory.
I have no way of opening the file (as we are still on 2018).
Hmmm sounds interesting. I would very much like to open the file to give it a try...
My bad... If you select "end trim" then you have the option to select the planes or simply use the flat surface of the 320mm members. One on each end.
Habib Ghalamkari wrote:
Fernando Castellanos wrote:
Hi Habib,
You need to use the trim/extend tool in SolidWorks:
Have a play around with it to see how it behaves.
Hope this helps!
F
Hi Fernando,
Sorry for not mentioning. I'd already test that one.
It gives me the following error.
Bodies do not trim each other completely. Please Check your input.
thanks.
I initially got the same error when trying to use the Trim/Extend function to cut off the Angle. You need to de-select "Allow extension", and then it works fine with selecting the edge shown as the Trimming Boundary.
Interesting Habib,, I'm not a weldment person (done very little). What I ended up doing is making a couple of planes off of the 320mm flat faces. Then used those planes for a split feature. Consumed those pesky extensions.
Fernando Castellanos & Dennis Bacon
Thanks for all your solutions.
I tried and both were excellent.
I was also able to follow Fernando's solution and do it without adding planes. (I selected the flat surface of angles instead.) Which makes my feature tree shorter.
Before accepting one of them as correct answer, I hope you don't mind asking another question.
Are these additional extensions ( I don't know what to call them) normal?
Is there any way to prevent them being created? (instead of trimming them)
Thanks again.
No worries
They can be caused by a number of things such as profile shape, number of connecting joints (ie. how many profiles are going into a point) trim order when you're creating the weldment and sometimes even the angle of the sketch. Best way to keep your tree short is to look at the trim order when you're creating the weldment. This will save you from having to use trims later on
The 'extensions' is normal. They are called 'coping'.
It's used to extend the angle, channel inside another one to fill up the profile.
In your case, its working as design but not what you want.
That's the different with Trim/Extend to face and bodies.
Million thanks for sharing your knowledge and experience.
Ok, so this editor is stupid and I cannot upload videos (for some reason...)
First, you need to create a reference plane on the edge of your profile:
Then, go to your trim/extend tool and input your bodies (change the trimming boundary to Face/Plane)
Discard the part you don't want to keep.
Should work