Dimensioning and constraints

[fade2blue]

When in 2d sketch mode I can not dimension or constrain my sketch to the default datum planes or axis(x,y,z). I have tried adding work planes coincident to them with no luck. (offset plane distance 0.0). I haven't found anything in the help files to shed light on this.

 

[rollupswx]

Project Geometry and select the desired origin plane or the origin Center Point. I suggest changing Application Options to Autoproject the Origin Center Point.

 

[yehlo1972]

U have to project the planes, axis or a point through project geometry.

 

[rollupswx]

Yes, do what yehlo1972 said.

 

[bilobaglen]

I have same problem & not sure if the answer is applicable.
eg: I create a cylinder extruded from the xy plane.
Then I add a hole to the face which is on the xy plane, the hole is not concentric to the cylinder so I need to dimension coordinates from planes xz & yz.
I don't seem to be able to do this, I cannot select the planes. Auto project is set in the application options.
I have just started with inventor after some years with Proe & Solidworks.

 

[rollupswx]

You could have used the Concentric placement method to place the hole in the beginning. What placement method did you use?
You could have also used the From Sketch placement method by first creating a sketch with a Point, Center Point.

My guess is that you are trying to use the Linear placement method which would no sooner work on the real physical part out on the shop floor than it will in Inventor as there are now linear edges to the part and it will not allow you to select the imaginary Origin workplanes.

Inventor works a bit differently than SolidWorks or Pro/E. Start the Hole command and click on the down arrow underneath Placement for options.

 

[aardvarkdw]

More or less reiterating what rollupswx said, when using the hole tool it is best to start a sketch and dimension to a centerpoint unless you are placing a concentric hole. Bilobaglen, in your case because you don't have any "linear" edges the linear hole placement command wont work. It will only select physical surfaces.

David

 

[bilobaglen]

Thanks rollupswx, I should have said that the hole is deliberately not concentric but I still wanted to relate the hole to the origin planes, just like you might in the shop if you started with a disc having a centre point plus a horizontal & vertical centre lines.
I did manage to make the hole with a sketch & cut & then I can apply ordinate dimensions from the origin point which does what was intended but perhaps not in the best way.
I still could not get the hole command to work the same way with any of the options. What I am trying to do seems so basic & I'm sure it will all make sense in a day or so.

 

[rollupswx]

Without seeing the part I think what you want to do is start a new sketch on the end of the cylinder. Project Geometry and select the axis planes or the Origin Center Point. Create a sketch point and dimension the offset to the projected cross or origin. Exit Sketch
Start the Hole command and the sketched point will automatically be selected as the hole location.

 

[bilobaglen]

rollupswx & aardvarkdw
With your help I have produced & dimensioned the hole using both the cut & the hole commands, many thanks.