Help needed with Solidworks 2013

[fractured]

I have just drawn a part that is cylindrical. It has a number off different diameters and lengths etc, but all have been drawn on the same axis, so every time I needed to add a different shaped cylinder I just started a new sketch on the end of the last cylinder and used the centre to start the new sketch- so pretty simple.

However, I now need to make a rectangular hole through the side of the cylinder. As each different part is a feature (extruded section to give length of cylinder) I am not sure how to create a new sketch on the side of the "feature" - ie, the side of the extruded cylinder.

Could anyone give me an idea of how to do this, or do I need to draw in a different way?

Thanks in advance for any help and advice.

Mick

 

[Martin-Sy]

Rather than sketching on a feature, can you sketch on the appropriate plane? ISTR you can do this in F360, not sure about SW tho.

 

[sako243]

No significant experience on solidworks but on Inventor you can create a new sketch plane parallel to an existing plane and coincident with the curve of the cylinder. Or you can just do an offset plane if you're happy with a fixed offset based on the radius of the cylinder.

From that plane you can create a new sketch for the rectangle.

 

[Erie Fred]

I have just drawn a part that is cylindrical. It has a number off different diameters and lengths etc, but all have been drawn on the same axis, so every time I needed to add a different shaped cylinder I just started a new sketch on the end of the last cylinder and used the centre to start the new sketch- so pretty simple.

However, I now need to make a rectangular hole through the side of the cylinder. As each different part is a feature (extruded section to give length of cylinder) I am not sure how to create a new sketch on the side of the "feature" - ie, the side of the extruded cylinder.

Could anyone give me an idea of how to do this, or do I need to draw in a different way?

Thanks in advance for any help and advice.

Mick

Why did you do it this way ?
I draw the side, and then revolve.

Either way, if you kept all your "circles" on the center of one of the axis, start a new sketch on a plane that intersects it.
Draw your rectangle, and then cut xtrude "thru all" in both directions.

 

[cr500dom]

Turn the planes on (Right Click on them in the history tree and select the eye) and then sketch on the plane, extrude your cut.
For future reference, if its a turned part its better to detail all the various diameters and lengths in one sketch (like a section view) and then revolve

 

[Erie Fred]

For future reference, if its a turned part its better to detail all the various diameters and lengths in one sketch (like a section view) and then revolve

Yup, I do shafts all the time, and by placing them as above, you can set relationships
between those diameters.
For example, a motor shaft has bearings. You can set the distance between the shoulders the bearing register on.
Change the other lengths & dia's all over the place as the design progresses, but those stay.

Just stacking one atop another, you would be constantly adjusting other lengths to keep those fits the same.

 

[cr500dom]

So your construction method was similar to this:


Note the history tree

Then turn on planes to sketch and cut rectangle:



Add chamfers and Fillet Rads, Note the history tree:



What I and others are proposing is this:



All the details in one easily modifiable sketch
Note the history tree now:



Sketch rectangle and extrude cut as before:



Now you have 2 features and only 2 sketches in the history tree as opposed to 9 features and also, dimensioned as it is, the main revolve, you can change the length of one element without affecting overall length or changing the others. so when you modify your sketch later, you can immediately see the knock on effect to the other sections


Hope that helps ?

 

[fractured]

Many thanks gents.

#cr500dom many thanks for the explanation which I tried to follow but I think cocked up. First thing I did was to draw the sketch for the cylindrical body but I also included the rectangle. I rotated the outline of the cylindrical parts and used the revolved boss feature to create it from the outline of the part - I did not select the rectangle as I did not want to form that as part of the cylindrical piece. I have now tried to use the extruded boss feature but it wont let me do this.

So on further looking at your explanation I see you mention 2 sketches. I presume this is so that the cylindrical part is on one sketch and the cut rectangle is on another - could you confirm this? So with this in mind, do I need to delete the rectangle from sketch 1 and create a second sketch for the rectangle?

Thanks for your help so far, it has been really useful. My problem is I have been used to 2D draughting with AutoCAD so I am struggling getting my thought process to focus on different sketches. I feel as soon as I can get cracked on that I can start moving forward as currently I just seem to sit and get frustrated.

ATB

Mick

 

[bricol]

Yup, I do shafts all the time, and by placing them as above, you can set relationships
between those diameters.
For example, a motor shaft has bearings. You can set the distance between the shoulders the bearing register on.
Change the other lengths & dia's all over the place as the design progresses, but those stay.

Just stacking one atop another, you would be constantly adjusting other lengths to keep those fits the same.

Exactly my approach too.

However, a colleague, who has been contracting since the mid-80's, trained/experienced in many industries, mainly aerospace, insists on the stacking cylinders approach - bugs the 'eck out of me. Proven by others to be an easy mistake to make - as you describe - extended one extrusion, failed to spot he needed to reduce another to keep the overall length the same. Few hundred components made . . . 12 installed, machine started . . . BANG . . .

 

[bricol]

Many thanks gents.

#cr500dom many thanks for the explanation which I tried to follow but I think cocked up. First thing I did was to draw the sketch for the cylindrical body but I also included the rectangle. I rotated the outline of the cylindrical parts and used the revolved boss feature to create it from the outline of the part - I did not select the rectangle as I did not want to form that as part of the cylindrical piece. I have now tried to use the extruded boss feature but it wont let me do this.

So on further looking at your explanation I see you mention 2 sketches. I presume this is so that the cylindrical part is on one sketch and the cut rectangle is on another - could you confirm this? So with this in mind, do I need to delete the rectangle from sketch 1 and create a second sketch for the rectangle?

Thanks for your help so far, it has been really useful. My problem is I have been used to 2D draughting with AutoCAD so I am struggling getting my thought process to focus on different sketches. I feel as soon as I can get cracked on that I can start moving forward as currently I just seem to sit and get frustrated.

ATB

Mick

It is difficult to get out of the mindset/thinking of 2D into 3D. I only commented yesterday to a colleague I knew it was one of his older models I was modifying - every single feature was detailed on one sketch, making work on it much harder than needed.

One feature - one sketch.

Sketch for the base feature - create the shape.
Sketch for child features, one for each - slots, holes, additional bosses etc.

 

[sako243]

I have now tried to use the extruded boss feature but it wont let me do this.

If Solidworks is like Inventor then once you've "used" the sketch then any bits within it are basically unavailable for further features to be created from them because it's a sort of 1:1 mapping between sketches and features. If you had selected the rectangle then you'd have ended up with a rectangular section being revolved around the axis.

What you need to do is create one sketch for the cylinder body and then create another sketch on the central plane / axis for the rectangular section to be punched through.

 

[mike os]

Always make simple sketches for an individual shape, body or feature

Then add features individually... ie a hole or series of similar holes, bosses etc then add another sketch for further detailing

Trying to make a part from a single or complex sketch always leads to issues if you need to modify

 

[cr500dom]

If Solidworks is like Inventor then once you've "used" the sketch then any bits within it are basically unavailable for further features to be created from them because it's a sort of 1:1 mapping between sketches and features. If you had selected the rectangle then you'd have ended up with a rectangular section being revolved around the axis.

What you need to do is create one sketch for the cylinder body and then create another sketch on the central plane / axis for the rectangular section to be punched through.

No in Solidworks you can use the same sketch for different elements, just select the regions you would like for that feature.
So if the OP has a sketch containing all the features, select the region for the revolve and complete that feature.
Then right click the sketch(Now absorbed in the feature) and show, keep i selected and just hit extruded cut, this should then allow you to select the rectangular cut out region and just use that (Or it does now, im not sure on 2013) even if it wont do that, you can just create another sketch and within that sketch you "Convert entities" and select the rectangle
That focuses / carries through the original sketch features to the new one.

You can use this feature to get really clever once you get your head around it.

When I am designing cylinderheads, I will create a skeleton part first which just has a load of geometry and sketches in it, cam centres, valve angles, port shapes, plug positions, injector positions etc
Many of these will be linked to one another via formulas or equations too.


Then I'll create an assembly, with this part in.
I'll create new parts within that assembly for cores and offsets for cutters etc, all of which will reference different sketches/features in the skeleton part.

Now if your valve angle changes, and you update the skeleton part, all of your other cores will reference that change and update to the new valve angle.
If you've done it right, then apart from a few fillets falling over in the models (Which should all be at the end of the tree anyway for that reason) you don't end up with the issue like Bricol says above.

 

[cr500dom]

Many thanks gents.

#cr500dom many thanks for the explanation which I tried to follow but I think cocked up. First thing I did was to draw the sketch for the cylindrical body but I also included the rectangle. I rotated the outline of the cylindrical parts and used the revolved boss feature to create it from the outline of the part - I did not select the rectangle as I did not want to form that as part of the cylindrical piece. I have now tried to use the extruded boss feature but it wont let me do this.

So on further looking at your explanation I see you mention 2 sketches. I presume this is so that the cylindrical part is on one sketch and the cut rectangle is on another - could you confirm this? So with this in mind, do I need to delete the rectangle from sketch 1 and create a second sketch for the rectangle?

Thanks for your help so far, it has been really useful. My problem is I have been used to 2D draughting with AutoCAD so I am struggling getting my thought process to focus on different sketches. I feel as soon as I can get cracked on that I can start moving forward as currently I just seem to sit and get frustrated.

ATB

Mick

Mick, what I would suggest is go into the help menu and open the tutorials, it is the best way to learn, honestly, a few hours working through those will set you up properly for using solidworks.
It is one of the best feature of the software.
The training is all embedded and it highlights where you need to click on the main screen as you hover over the symbol / instruction in the tutorial.

 

[Erie Fred]

Using one sketch multiple times, In Inventor you click on that sketch (in the tree on the left) and right click
"Share Sketch"
It flags it differently, and is now available for more work, like the cut extrude you want to do.