Grooves in Round Bar

[English Lad]

Novice Question I'm Afraid

 

I want to put a series of grooves into a round bar instead of knurling the surface how do I do this?

 

I extruded the round section by creating the circle on the end of square bar.

 

Picture attached of what I am trying to do.

 

Paul

[JD Mather]

Sounds like you want to do a Revolve-Cut.

[English Lad]

Sounds like you want to do a Revolve-Cut.

 

Hi JD,

 

Just looked that up with your pointer but how do I get it to revolve around it? Do I need to draw the sketch as a 3D sketch?

 

Paul

[JD Mather]

Attach your file here. Have you gone through the Help>Tutorials?

[English Lad]

Attach your file here. Have you gone through the Help>Tutorials?

 

It wont let me upload the file as its 318K

 

Can't see anything in the Solidworks tutorials that is similar

[shift1313]

Are you cutting a groove for a C-clip or are you cutting one longitudinal to the shaft for a keyway?

 

for the c-clip you will need a 2d sketch. You will draw a cross section of your groove(square probably) and a reference line that will be located at the center of your shaft for this groove to revolve around. This sketch should be on a plane centered on your shaft. Depending on how the original part was drawn, one of the standard planes should do. if not you will need to create one.

[JD Mather]

It wont let me upload the file as its 318K.

 

Drag the end marker of the feature history tree up to hide all features in the graphics window. (assuming you are using 2007 or later that will let you save in a rolled up state)

Save the file in a rolled up state.

In Windows Explorer right click on the file name and select Send to Compressed (zipped) Folder. The resulting *.zip file should now be much much smaller.

[English Lad]

Hi all,

 

Thanks for all your help.

 

I don't know if how I achieved it was the correct way but this is what I did....

 

Created a 3d Sketch so that I had a centre line, then created plane based upon the centre line and face 1 set it to perpendicular (This put the plane centrally through the component).

 

Created a circle on the plane and then did a revolve cut followed by a linear pattern to repeat it.

 

File attached in SW2010 format.

tapwrench_part1.zip

[DannyB]

Ahh, your modelling a tap wrench. If what you achieved was ok, thats fine. But tap wreches like that, normally have diamond knurled shafts. You could put this on as an appearance on the shaft. You do this by changing the appearance of the face to a patterend one and adjust it until it looked right.

[English Lad]

Ahh, your modelling a tap wrench. If what you achieved was ok, thats fine. But tap wreches like that, normally have diamond knurled shafts. You could put this on as an appearance on the shaft. You do this by changing the appearance of the face to a patterend one and adjust it until it looked right.

 

I could have knurled it but there are many tap wrenches that have plain handles as well.

[shift1313]

Sorry but i have 2009 so i cant open your drawing. I dont see the need for a 3d sketch though. Here is how i approached the model.

 

First the sketch for the main block. You can see the origin is at the midpoint of the left edge. This also puts both holes center points horizontal with this. I could have done a little more with symmetry for the twho holes but i just added a dimension.

 

In the second pic you can see all 3 standard work planes are centered on my block. The extrusion i did as a Mid Plane rather than blind to keep my front and top plane centered. This made it easy to extrude the handle as the origin was the locator for my circle.

 

For the groove you can see my sketch. The dashed line is a horizontal(infinate length) reference line from the origin. This will be used as my revolve axis.

 

Image 5 shows a preview of the revolve/cut

 

Image 6 just shows a close up view of the cut(G for Magnifying glass).

[English Lad]

Hi Shift (Matt),

 

My planes are not central to the sketch hence why I had trouble.

 

I just created the sketch and extruded it and then placed a circle on the square end and extruded that.

 

I have just trid to replicate getting the planes to be central and I failed....

 

Draw sketch on front plane origin is bottom left corner of sketch, extrude choosing mid plane.

 

Front plane is correct through middle, but top plane is on a side, right plane is as you would expect on the right side.

 

Question.... How do I get the other plane (top) central? Does it depend on which plane you draw the sketch?

 

Paul

[shift1313]

Hey paul, take a look at the first image i uploaded. the origin(red) is at the mid point of my initial rectangle. If you select your vertical line and the origin point you can choose midpoint as one of the relations.

 

I would strongly recommend taking this approach to modeling as it will simplify everything from updates, plane creation and being able to use symmetry about the origin. However with your model you can still follow the same procedure by creating a work plane that is centered.

[English Lad]

I must be doing something wrong as if I click the line I do not get the option for mid point...

 

Do I need to hold a key down or something to select the red origin at the same time:oops:

[shift1313]

It looks as if you started your sketch at the origin so you already have a coincident constraint with origin. You can see the green icon just under the origin. Either start drawing your rectangle away from the origin or delete this constraint and then add the midpoint one.

[shift1313]

just as another note. when sketching with auto-constraints turned on, if there is a point where you do not want a constraint applied you can hold down the ctrl key(i think it was ctrl) this temporarily turns auto-constraints off while holding the key.

[DannyB]

If you pick a corner rectangle you need to set midpoints to the horizontal and vertical lines for it to be symmetrical about the origin. Or you could select the centre rectangle from the drop down in the sketch toolbar. This way you start from the origin, outwards and it's symmetrical.