I've made a sketch (attached) where I'm attempting to offset the outermost loop by a certain distance. When I try the offset tool, despite the fact that the "Loop Select" is checked, it wont allow me to select the whole loop, but ony parts of the loop at a time. I know it's a closed loop because I'm able to extrude the sketch with no problems. I can't seem to figure this out search of the forum didn't turn anything up. Any help would be appreciated. Thanks. - AJ
I didn't take the time to diagnose your sketch for the offset issue, because I think there is a more important issue to discuss, and that is the overall approach. First off, great job creating the sketch and getting it fully constrained. But I think you can create your part more quickly and easily by going about it a bit differently. Have a look at the way I approach your part in this video and you'll notice that it comes together without fighting sketch geometry and when I get to the offset feature at the end, the profile offsets easily.
You'll notice that rather than building one complex base sketch to house all of the features, I can create this part more easily and quickly by creating a series of simple sketches from which I build simple features that all add up to a complex part (simple sketches + simple features = complex part). Approaching solid modeling in this way will keep you from having issues as you've had with the offset, and you'll spend more time designing and less time diagnosing issues with sketches.
Here is more reading on simple sketches:
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
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its does not work....
the solution is offset it individually and apply coincident contraint....
i have attached it....
Make sure you have your software up to date. There was a hotfix for this in 2012. I am up to date and this worked fine for me on the offset.
Thanks curtis. I'm just a beginner/student so I'm learning. I was hoping to built a base sketch from which two parts would be built that have complementary contrours on the faces that are opposite of each other (hard to explain). That's why I was hoping I could build one sketch which would form the basis of both parts, hence the complexity. I like your approach though and will implement that where ever possible.
If that is your intention then you are not doing anything wrong. Having a complex sketch is not a bad thing and using multi body solids is a great way to go with complex contours. I think Curtis just wants you to see good general modeling practice first and then you can apply that to your more complex design.
You should look at multibody solids though for your intent with this model.
Hi Mark. I'm running a student copy of 2011 Professional. I found the right update (http://usa.autodesk.com/adsk/servlet/ps/dl/item?si
That Hotfix relates to Projected Geometry - not what you have.
I suspect you are missing some intended tangents in your sketch - and do the offset before adding construction lines.
But there might be a better way alltogether - offset or shell from the solid geometry rather than sketch.
Find the Service Packs for your release and install.
Finish the part(s) any way you can and then attach here for alternative techinques.
What Curtis suggests is good modelling practice but there are always times where it is desirable to add your features in the sketch. The problem is all your symmetry constraints and duplicated lines. I would start by drawing it 'freehand' then constrain and dimension. If you draw a straight line then click the end point and drag away you can create a tangent arc. Use this to draw your full profile in one go then utilise equal constraints instead of symmetry. I would still add the holes after the profile has been extruded.