I thought that I would go back to sketching basics in this blog and look at five tips that you may have missed if you were self-taught or, even if you are an experienced user, you may have forgotten about. Either way, I hope that these might help you be a little more efficient in the Inventor sketch environment.
#1 Scaling in a Sketch
Here's something you might not realize in an Inventor sketch! When you add your very first general dimension (not one created automatically), that dimension sets the scale for all sketch entities in the sketch. Change its value before finalizing the placement of the dimension, and all the other sketch entities in the sketch will adjust in size based on the change made to the first dimension value. So, if a sketched line was approximately 1 and it was dimensioned and immediately modified to 2, all other sketched entities in the sketch will be doubled in size. But as soon as you add in a second dimension, automatic scaling stops.
If you don’t like the auto-scaling feature, you can change a setting in your Application Options to prevent it from happening going forward.
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In the Tools tab>Options panel, select Application Options.
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In the Application Options dialog box, on the Sketch tab, clear the Auto-scale sketch geometries on initial dimension option.
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Click OK.
#2 Projecting Construction Entities
This is a tip that I had forgotten about, but will get back to using again. When you project geometry into a sketch, it is automatically projected as a solid sketched entity. If you plan on using the projected entity as a construction entity, you can press and hold <Shift> when selecting the entity to immediately project it as construction (yellow dashed line). This prevents you from having to convert the entity to a construction entity after it has been projected – saving you a few steps!
#3 Adding Missing Constraints
The 
(Automatic Dimensions and Constraints) command can be convenient to automatically assign dimensions in a sketch. However, personally I find I don’t use it to add all dimensions, because I want to fully control the intent of my dimension scheme. Where I do use this option is when I can’t seem to figure out why my sketch is not fully constrained! In these situations, I use the tool to automatically apply the missing dimensions and constraints, see where in the sketch they were added, Remove them, and then assign them in a way that works with my design intent. The Auto Dimension dialog box even allows you to decide whether you want to know where dimensions or constraints are needed.
Alternatively, I have also used the 
(Show Degrees of Freedom) option in the Status Bar to reveal which entities can move, as shown below. This can help you determine where additional constraints and dimensions are required to fully constrain the sketch. In this case, a vertical perpendicular constraint could be added to the 5 in. entity to fully locate the sketch. Once the sketch is fully constrained, all degrees of freedom symbols are cleared.
#4 Showing Constraints
In some situations, you may have a fully constrained sketch and yet are unable to assign a dimension that you need.
In these cases, it is generally because of constraints that have automatically been assigned during sketching without you being aware. To review the constraints that are assigned in the sketch, you need to show them. There are a few different ways to do this. Consider using any of the following:
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In the Status Bar, click
(Show All Constraints) to display ALL applied constraints in the sketch. Click 
(Hide All Constraints) to remove them from the display.
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Using your keyboard, you can press <F8> to display ALL the constraints. Press <F9> to remove them from the display.
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In the ribbon, in the Constraints panel, click
( Show Constraints) and select entities in the sketch to display their constraints. Alternatively, you can draw a selection box around all the entities that you want to display constraints for. When constraints are displayed using this method, click (Hide All Constraints) in the Status Bar to remove them from the display.
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In the graphics window, you can hover the cursor on a sketched entity to temporarily display its constraint symbols. Moving your cursor away from the entity will clear their display.
#5 Inferring Sketch Constraints
Everyone familiar with sketching in Inventor knows that constraints can be explicitly assigned to sketched entities using the constraint options in the ribbon, and most also understand that, by default, constraints are assigned as entities are sketched. But did you know that you can customize which constraints are inferred as you sketch? This can be quite helpful to customize and control what’s happening as you sketch and is recommended as you become more familiar with sketching. To control which constraints are inferred while sketching, in the Sketch tab>Constrain panel, click 
(Constraint Settings), then select the Inference tab.
By default (as shown above), constraints are inferred and all constraint types listed are enabled for inference. You can enable/disable the constraints that are to be inferred, as required. Or you can completely disable allowing inference at all while sketching by clearing the Infer constraints option.
A few other helpful tips:
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When sketching geometry, you can also press and hold <Ctrl> to override the settings during the sketching process.
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The software automatically determines which existing reference and inferred constraint type are assigned to an entity as it is being sketched. If the inferred constraint is not as required, hover the cursor over a different entity in the sketch to infer a different constraint type and then place the entity.
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You can change the priority of whether parallel/perpendicular or horizontal/vertical constraints are assigned, which can be helpful if you are sketching at angles to the origin planes.
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The Persist constraints option can also be useful. When this is enabled, it infers the constraint during sketching AND also assigns the constraint to the sketch. If this option is disabled, it infers the constraint during sketching but DOES NOT assign the constraint to the sketch.
I hope that these sketching tips help you become more efficient with your sketching.
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