hello sir my angle bar structural not proper angle bar length 1000 mm this problem actual is 900 mm 1000-50-50=900mm
plz hel actual size 900 mm
as Cas Adin pointed out-
you need to use the "Trim/Extend" (circled)
feature for matching machined parts/corners
(see att.pic below)
I've attached my take on your part, SW12-
just to show a different approach-
use the roll-back bar to inspect the build
hope this helps- have a good'n - kelef
Your vertical legs need to be Trimmed. Use the Trim/Extend in your Weldment Tab.
Two valid answers already provided, but adding my 2c..
I would only use the Trim/Extend command when modifying Structural Member bodies from different profile shapes. It appears that your Vertical and Horizontal bodies share the same profile. From this, you can assign each orientation of the same profile as separate groups within the same Structural Member feature. Including multiple intersecting bodies in the same Structural Member allows for automatic trimming, and/or customization through using the Purple circles at each junction to prioritize which item is coped into which unmodified bodies.
If trimming a Plate entity from an Angle body it's mounted to, or coping an Angle into a Channel face (dissimilar profiles), then I'd use Trim/Extend.
THANKS SIR BUT I TRY BUT SOME PROBLEM YOU NEED THE SOME HELP VIDEO TO ME REPLY
I tried making a rough video showing how to do this, but encountered what I think are similar errors. These images should show what you may be encountering. Note I do not have metric profiles installed, but was able to edit your features without problem.
Trim/Extend upon separate SM features (both top and bottom trim, only bottom shown) :
One SM using automatic trim (both top and bottom trim, only bottom shown) :
These stubs at the end result from both automatic trim and feature trim. They are resulting in cut length not = 900.
Here's what did work. I rolled back to create a plane parallel to Top and coincident with upper vertex of 3DSketch2. I sketched on that plane (not a face which can change or disappear), converting horizontal line entities from 3DSketch2. I repeated this on Top Plane located at part's bottom. I used Extruded Cut feature (twice, top and bottom) to cut 50mm blind with Feature Scope of only Selected bodies, where only the vertical pieces were selected. I resulted in 900 cut length as shown. :
Compound angle coping at 3-way corners often have this small artifact shown in the 1st two images. I tried several options available only in the Trim/Extend command (because there are a few), but could not find a setting to result in a clean square end cut like third image. I had hoped to find something instructive there, but ended up doing it the harder manual way instead with actual cuts upon selected bodies. My fabricators can ignore this flaw, but it will affect your cut-lists, which likely is the issue I've shown here.
I don't expect this was the solution you wanted. I'd also expect some 'common sense' solution in weldment trim results, but I've learned to rely on edge dimensions in my fab drawings instead of cut lists for this reason. Maybe someone else can help better on these last two paragraphs by showing which Trim setting achieves a square cut not a curved stub poking out.
Is this the detailed nature of your error with others' advice, or am I misunderstanding? I cannot continue to help without a better understanding of your issue and computing environment.
Last desperate workaround.. sometimes I resort to this because 3dSketches are very flexible like that. There's always more than one way to get it done. Edit 3DSketch, use Split Entities sketch command to break the verticals into three lengths, set upper and lower related as equal (length), then dimension one to 50mm. (1st image below). This results in 2nd image below, where SM3 is ill defined because the short piece was the stub not the long part. Edit SM3, and make sure to select new segments to add to a group before deselecting the wrong segment, which maintains its settings without resetting them. 3rd image below is result. (Note that if you had made any segment in the sketch a construction line, then it would not be able to be used as a weldment path and would really break the SM3's definition and require full redefinition. Sometimes I'll use a construction line to establish relations to a mounting axis or cylindrical tangent face or such within my sketch, then define other useful portions of the sketch from that.)
You must use one "Structural Member"
In this way, you don't need to use "Trim/Extend" command.
I always use one "Structural Member" and never use "Trim/Extend", I never need.
I agree with the single member statement (proper modeling is always preferred), however the trim/extend is a faster resolution to resolve the issue.
Yes, faster. But, when to make revision is necessary, it will be very hard to do.
If you make revision a lot or "save as copy", you must not use "Trim/Extend".
Sometimes, If even use one "Structural Member", your profile can be nested.
In the face of such a situation; you must edit future(structural member) and click the corner and change trim order.
And our cage is ready.
I agree with the single member statement, proper modeling is always preferred.
But I have cases where I have 2" angle nesting to 1.25" HSS that is attached to 1.25" angle. Trim is the only option then. But when using a single type of member it is always easiest to set it up properly with a single feature whenever possible.
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