JBEANGE Posted June 7, 2020 Share Posted June 7, 2020 Hi All, Does anyone have any tricks for putting on hole trough two pieces of sheet metal? I currently drag in a cut cylinder into the first material then have to drag another on into the second piece of material which is extremely time consuming... TIA Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted June 7, 2020 Share Posted June 7, 2020 Right-click and drag-and-drop a hole on to one sheet metal. Select assembly Feature. Once created and positioned, right-click on the assembly feature and select create Part Feature. Other option is to drop a solid cylinder part into the scene and position it. Select on one sheet metal and the cylinder and select Cut Sheet Metal. Repeat on the other part. Quote Link to comment Share on other sites More sharing options...
JBEANGE Posted June 8, 2020 Author Share Posted June 8, 2020 Thanks Cary, My IronCad doesn't appear to have the "create part feature" mine ends at Intellishape Properties... Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted June 8, 2020 Share Posted June 8, 2020 Are you sure you dropped as an assembly feature? It should be a white highlight (not yellow). If it is yellow, it will not have those options. Quote Link to comment Share on other sites More sharing options...
Malcolm Crowe Posted June 8, 2020 Share Posted June 8, 2020 Attached is a demonstration video that might help identify what you might be missing. Malcolm Assembly Features - Holes through Sheet Metal Parts.mp4 Quote Link to comment Share on other sites More sharing options...
HDEAR Posted June 10, 2020 Share Posted June 10, 2020 (edited) Thanks Malcolm. After applying the assembly features and prior to 'Create Part', you can adjust the hole size and you can also adjust the position and both sheets will reflect that change. If you complete an unfold on either sheet, that hole you created through both sheets, does not transfer onto the unfolded sheets. After completing the 'Create part' however, both sheets will reflect the hole that was made on their respective unfolds, however there's now no chance to alter the hole size or have it follow any positional change. Is there any way that after 'Create part' is made, that any size or positional change can be made that is reflective on both sheets? Harley Edited June 10, 2020 by HDEAR Quote Link to comment Share on other sites More sharing options...
HDEAR Posted June 10, 2020 Share Posted June 10, 2020 (edited) Here's one way to do it. You can create the bends, mitre bends, whatever on your first plate ( blue in the video ) Add the holes on the flange that you want mirrored and followed. When you create the other plate onto which you wish to have your holes mirrored, you have to make sure that you have stock to mirror onto rather than bends. So on the orange sheet, you'll see I knocked the bend down to zero length, and added 'Add stock' This then allows allows you to edit that 'Add stock' ( or any stock for that matter ) and use 'Project constraint'. Once done, any hole size changes and even positional changes on the master sheet will transfer transfer to the slave sheet. A bit fiddly, but it is a method that works. Sorry about the end of my video, I ma having trouble stopping Active Presenter with the CTRL-END function - it seems real finnicky! Harley Holes through sheetmetal - resize and follow.mp4 Edited June 10, 2020 by HDEAR Quote Link to comment Share on other sites More sharing options...
Malcolm Crowe Posted June 10, 2020 Share Posted June 10, 2020 Hi Harley, While we are on the topic, here are a couple of options available for editing holes that have been created from "Assembly Features". 1. The size of the "Created Part Features" can't be changed (that I can see), but their position and number can be edited using the TriBall. Select at the intellishape level by holding down the "Alt" key when clicking. In the attached video I am holding down both the "Alt and "Shift" keys as I am selecting multiple intellishapes. 2. Delete the existing "Created Part Features", and recreate new ones using the original "Assembly Features". In the attached video I have left the original Assembly Features in place. When the "Create Part Feature" tool is used, the parts are removed from the "scope" of the "Assembly Features". In the attached video I select "Edit Assembly Feature Scope". With the dialog box open I select the parts in the scene (while holding down "Ctrl" + "Shift"). Once selected I can click on the "Add Parts" button. With the Assembly Feature now being applied to these parts again I can edit the size, number, and position of the feature. When done the "Create Part Feature" tool can then be used again to apply to the individual parts. Malcolm Assembly Features - Editing Holes through Sheet Metal Parts 1.mp4 Assembly Features - Editing Holes through Sheet Metal Parts 2.mp4 Quote Link to comment Share on other sites More sharing options...
Malcolm Crowe Posted June 10, 2020 Share Posted June 10, 2020 The attached video demonstrates the same as above but with "Patterned" holes (which is a more efficient and easier to edit method). Malcolm Assembly Features - Patterned Holes through Sheet Metal Parts.mp4 Quote Link to comment Share on other sites More sharing options...
HDEAR Posted June 11, 2020 Share Posted June 11, 2020 (edited) Thanks Malcolm. I sometimes avoid Patterned features as these don't copy and paste unless put into an assembly ( as far as I can see ) but I agree, when you use them, they're much easier to modify. Good advice from you once again Harley Edited June 11, 2020 by HDEAR Quote Link to comment Share on other sites More sharing options...
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