Uneven surface

[Anonymous]

This is a trial. This model’s bottom surface is uneven. I want to make 4 similar chamfers on 4 surfaces. Start 2D Sketch command is selecting only one surface at a time. I know one method is using Work Plane command then I can select all 4 surfaces together.

I wish to know whether there is any method to use PLANES in the left side of browser. Because XZ plane is highlighting the entire surface.

 

[JDMather]

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@Anonymous wrote:

 ...Start 2D Sketch command is selecting only one surface at a time. I know one method is using Work Plane command then I can select all 4 surfaces together. 

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You should have stopped with Sketch1 - it is not fully constrained.

I recommend that you sign up for a class on using geometry.

You can only start a sketch on a plane.

A planar part face is a plane.

You do not need to select multiple faces to define one sketch plane.

[Anonymous]

Now it is fully constrained. I attach the file.

[Anonymous]

So what is the usage of this plan? It is highly appreciated if you can explain with example.

[JDMather]

Use the origin workplanes if possible.  (They can't be deleted - rock solid foundation.)

If you can't use the origin planes then create a plane offset from the origin plane

or

use a part face.  (The part face can be deleted - so this isn't rock solid foundation, but if you know the part face will not be deleted in a future edit - then it is fine to use the part face.)

Does your instructor teach you anything in this class?

[Anonymous]

My instructor ask me to use array command to create 4 chamfers in a one shot.

[mcgyvr]

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@Anonymous wrote:
My instructor ask me to use array command to create 4 chamfers in a one shot.

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And what did he/she say when you said it wasn't working and asked them for assistance?

[mcgyvr]

and why are you even worried about creating sketches for chamfers or an array?

You don't need a sketch for a chamfer or an array..

And you can't just array chamfers either.. You can array an extrusion and chamfers applied to it but you cannot array JUST chamfers..

[JDMather]

When you get it finished - attach your file here and someone will show you how it should have been done (the easy way).

[mcgyvr]

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@Anonymous wrote:
When you get it finished - attach your file here and someone will show you how it should have been done (the easy way).

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Isn't that his instructors job 

From his questions so far its clear his instructor is absolutely useless..

[Anonymous]

I didn't try my instructor method. Create one chamfer and duplicate it as you need, this may be the my instructor's method.

[Anonymous]

Here we are. I have created 4 chamfers using my instructor's array method.

[mcgyvr]

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@Anonymous wrote:

Here we are. I have created 4 chamfers using my instructor's array method.

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You should have said you wanted to make a "chamfered hole" not just a chamfer in your original post (actually you probably should have called it a "countersunk hole"..)

Note there is a difference in "chamfer" and a "countersink" when applied to a hole..

A "chamfer" when applied to a hole is used to allow a pin or similar to fit into the hole easier or just to eliminate the sharp edge and as such diameter and angle tolerances aren't as critical.

A "countersink" when applied to a hole is to serve as a bearing surface for a flat head fastener and requires greater accuracy vs a chamfer... 

But since you didn't even include the word "hole" we got confused as to what you wanted..

This whole time I thought you wanted to do this which is a "chamfer"..

[Anonymous]

Thank you for your explanation.

[RobSinglehurst]

I've attached a modified version of your part with the part centred around the origin workplanes and then just using Mirror features instead of the Rectangular Array - much easier to modify in the future if you need to re-use it. I also removed a horizontal line in your first sketch to make it obvious which is the loop to extrude.

Centering on the workplanes makes the part much easier to constrain in an assembly as you will just constrain to the part origin workplanes which are always there.

[Anonymous]

Thank you for your help.

You begin the model from scratch. You place the origin to the middle point of the model. I wish to know whether it possible to move my model’s middle point to origin. I have attached the copy of my original model.

I asking this merely to explore the method of moving the model.  

[RobSinglehurst]

I used your model. Don't think of in terms of moving the part origin - more like moving the geometry in relation to the part origin.

I edited Sketch1 so that the projected part origin was vertically aligned to the midpoint of the raised line. I then turned the Extrusion into a Symmetric Extrusion (I nearly always use this option as then you don't have to extrude in the correct direction). 

I then edited Sketch2 in the same way and turned this Extrusion into a Cut All instead of a set distance as then this will take care of any future changes to the model.

In Sketch 6 I deleted the lines and directly dimensioned from the projected edges to the centre point of the circle. I only ever project the actual geometry I need for the sketch - less errors if changes are made at a later date higher up the 

Finally deleted the Rectangular Pattern and used the 2 x  Mirror Features instead - no need for any parameters etc once everything is modelled symmetrically.

[mcgyvr]

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@Anonymous wrote:

Thank you for your help.

You begin the model from scratch. You place the origin to the middle point of the model. I wish to know whether it possible to move my model’s middle point to origin. I have attached the copy of my original model.

I asking this merely to explore the method of moving the model.  

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Simply edit the first sketch and move the geometry to be centered on the center point..

If modeled correctly all other sketches/features should update automatically..

[Anonymous]

I adopt your method but other sketches/features didn’t update automatically. I am going to try again. May be the error in moving the geometry.

[mcgyvr]

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@Anonymous wrote:
I adopt your method but other sketches/features didn’t update automatically. I am going to try again. May be the error in moving the geometry.

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Worked just fine for me..

I edited your first sketch.. Removed one constraint to allow the sketch to move.. projected the center point and added horizontal and vertical constraints to center the sketch around the center point.. Then finished the sketch and eveything updated properly..