DRAFFERTY Posted October 10, 2017 Share Posted October 10, 2017 Hi All, I'm new to this forum, but the answer to this question has been bugging me for a while. I'm quite new to Ironcad, and I've only been using it since February. So there is a lot of tricks I haven't learnt yet. My problem has been that when creating 2D Shape sketches with larger assemblies with different parts etc. I have yet to find an easy way to hide the obstructive assemblies/parts. As I have the most experience with Catia, I'm wondering if there is a similar solution in Ironcad. In Catia, when in sketch mode with a plane that is inside of a part, you are able with the push of a button to "cut away" the part which obstructs the view in front of the plane. This also hides other assemblies etc and when pushing it again it show them once again immediately. The reason I need this is because sometimes I have to draw on large assemblies and parts and I need the parts visible in order to sketch their "outlines", but only behind the plane I'm currently trying to sketch on. I would like to thank replies beforehand. Regards, Dylan Quote Link to comment Share on other sites More sharing options...
Mike Hatch Posted October 10, 2017 Share Posted October 10, 2017 My problem has been that when creating 2D Shape sketches with larger assemblies with different parts etc. I have yet to find an easy way to hide the obstructive assemblies/parts. As I have the most experience with Catia, I'm wondering if there is a similar solution in Ironcad. In Catia, when in sketch mode with a plane that is inside of a part, you are able with the push of a button to "cut away" the part which obstructs the view in front of the plane. This also hides other assemblies etc and when pushing it again it show them once again immediately. 46008[/snapback] You can hide and un-hide parts, you can suppress and un-suppress parts, you can select an individual face and change its transparency, you could drop a surface onto a face from the glass catalog, I'm not sure if any of these give you what you want though. For me hiding and suppressing has always done what I needed when sketching in large assemblies, I don't believe you can change the hiding one a sketch has been started though. I'd also be interested to know if there is a single key type of "cut away" function as you describe in Catia. Mike. Quote Link to comment Share on other sites More sharing options...
jolizon590016 Posted October 10, 2017 Share Posted October 10, 2017 There is feature in Tools called Section Part/Assembly. First select Parts/Assembly from the scene or Scene Tree/browser. Go to Tools, click Section Part/Assembly and select the Selection Tool Type from the list like Block. Go to Section Options>Define Section Tool to position the desired block to cut away. Quote Link to comment Share on other sites More sharing options...
DRAFFERTY Posted October 10, 2017 Author Share Posted October 10, 2017 There is feature in Tools called Section Part/Assembly. First select Parts/Assembly from the scene or Scene Tree/browser. Go to Tools, click Section Part/Assembly and select the Selection Tool Type from the list like Block. Go to Section Options>Define Section Tool to position the desired block to cut away. 46010[/snapback] Thank you this is what I was looking for Makes life a lot easier. Quote Link to comment Share on other sites More sharing options...
Robert Andersson Posted October 10, 2017 Share Posted October 10, 2017 In addition, you can also Right Drag a block from the Shape catalog and drop it on some part. Then select option "Drop As Assembly Feature" and "AllAssy/ parts...". That block will now remove volume from all parts. This feature will show up in the Scene browser also where its scoop can be edited. Quote Link to comment Share on other sites More sharing options...
tlehnhaeuser Posted October 10, 2017 Share Posted October 10, 2017 You also have a various hide commands while in the Sketch mode. Attached is a video, although not a really a good example, maybe you get the idea. Tom Quote Link to comment Share on other sites More sharing options...
Cary OConnor Posted October 10, 2017 Share Posted October 10, 2017 Note: If you use the section tool mentioned above, you can right-click on the section plane and create a Section Profile (Sketch) as a starting point. Basically whatever is cut by the section will be placed into a 2D Sketch. Then you can modify the sketch to add whatever else you need. Cary Quote Link to comment Share on other sites More sharing options...
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