3D cad design sequence

[Jasonb]

I quite often do a section of the assembly which not only makes it easier to assemble the "inside" parts but once you start moving things about you can see where say the piston is at TDC and BDC. I'm fairly sure Atom has this, if you go to inspect along the top and then click precise section you can put the section on what plane you like and then click the items to section. Once it's in the tree on the left right click to make the section visible or not.

Another option is to have a few sub assemblies, this could be piston - wrist pin and conrod. You then go to "insert design" and choose the assembly rather than an individual part. You would then just need to set piston concentric to bore and big end concentric to crank pin.

 

[Bentwings]

the section view is a good idea I think I seem to remember solid works having what I called “ hall way view where you could view as if you were standing inside the model as I recal perspective had to be changed a little I haven’t got to that point yet. I’m still exploring what is installed on the system I’m using
I quite often do a section of the assembly which not only makes it easier to assemble the "inside" parts but once you start moving things about you can see where say the piston is at TDC and BDC. I'm fairly sure Atom has this, if you go to inspect along the top and then click precise section you can put the section on what plane you like and then click the items to section. Once it's in the tree on the left right click to make the section visible or not.

Another option is to have a few sub assemblies, this could be piston - wrist pin and conrod. You then go to "insert design" and choose the assembly rather than an individual part. You would then just need to set piston concentric to bore and big end concentric to crank pin.

 

[Richard Hed]

OK Slowly learning here. I got enough parts to get started so I tried to make an assembly. After a lot of trial and error I finally got some thing together. I am finding that constraints are both a useful tool and very easy to get the wrong constraints. Try inserting a new part and then find out that previous constraints do not let you do what you want to do. That means go searching for the previous constraints and find the ones which turned red and then modify them or delete them. For instance I positioned the piston in the correct center and rotation to the cylinder and then tried to move the piston to be concentric to the connecting rod wrist pin hole and when I move it it sent the cylinder down inside of the crankcase. I keep discovering things which make life easier. For instance trying to locate the wrist pin hole in the connecting rod is difficult because it is hidden behind the cylinder. I was going through the connecting rod tree until I found the right feature until I found that I can hide the cylinder to find the correct feature.

I have to do some more playing around with colors and opacity etc to have thing show without making them too dense or disappear entirely. Words of wisdom from experienced users are appreciated.

I also want to try animating things to see what happens when the crankshaft turns. I don't want to get too far down the line on the assembly because I am sure that I am going to have a similar problem of something having the wrong constraint which will not let the assembly turn.

Thanks to those who have given me advice on this thread.


View attachment 142076

sounds to me like you got further than me in how to use it.

 

[Richard Hed]

I quite often do a section of the assembly which not only makes it easier to assemble the "inside" parts but once you start moving things about you can see where say the piston is at TDC and BDC. I'm fairly sure Atom has this, if you go to inspect along the top and then click precise section you can put the section on what plane you like and then click the items to section. Once it's in the tree on the left right click to make the section visible or not.

Another option is to have a few sub assemblies, this could be piston - wrist pin and conrod. You then go to "insert design" and choose the assembly rather than an individual part. You would then just need to set piston concentric to bore and big end concentric to crank pin.

Do you have Atom? If so, how do you section a dwg then keep drawing? THis is all new to me--will have to try it. Geez loueez, I've been using Atom for a year and even Gordon has surpassed me in his ability to use it.

 

[Jasonb]

For an individual part or an assembly you do as I said above, go to "inspect" along the top black bar and then click "precise section"

If you want to put a section on a "working drawing" then it's the same as pro which I have get your basic elevations up on the screen and then along the top select "sheets & views" and from that "section" As you bring the mouse back over the working area you will get the first of several prompt, just follow these to choose the elevation to section, direction and where to place the section on the sheet.

 

[johnmcc69]

That's AWESOME Gordon! You're catching on! I'm glad you're sticking it out.

As Jason mentions, instead of assembling ALL the individual parts, create some sub-assemblies & then assemble those into your model. Please understand I've never ran Alibre, & can only comment on a "Workflow" I'm familiar with. I would typically create an assembly that would include the piston, wrist pin, connecting rod, bearing, & cap & assemble that sub-assembly into my "Top Level Assy.". When you get "Farther" down the road you'll understand this better. In the file I'm posting, it all looks like just a "few" parts right? Well, all the sub-assemblies are broken down & deatailed (This cuts down on my BOM showing a 'bazillion individual parts...

 

[johnmcc69]

(Duplicate post deleted...)

 

[johnmcc69]

Jason also mentions about sections & hiding parts. In my software (Pro-E), I can click on a part, right click & hide it. This helps immensely when in big assemblies. You'll figure this all out...

Gordon, my first 3D CAD project was a little oscillator from "Little Machine Shop", I can't find those now, but it was very helpful.

It certainly looks like you're doing a good job though, please keep us updated & post your progress. & most importantly, have fun!

Thanks to all of you for responses, I know I've learned a thing or two..

A big THANKS to Jason for his input, I "Threw him under the bus" when I put him on the spot. & I thank you sir.

John

 

[Jasonb]

Although I don't use it much Alibre also has the "hide" option in assembly. Either right click the part on the screen or down the tree then click hide from the drop down list, you will need to do the same to bring it back but can only do that down the tree as it won't be on the screen to click

 

[Richard Hed]

For an individual part or an assembly you do as I said above, go to "inspect" along the top black bar and then click "precise section"

If you want to put a section on a "working drawing" then it's the same as pro which I have get your basic elevations up on the screen and then along the top select "sheets & views" and from that "section" As you bring the mouse back over the working area you will get the first of several prompt, just follow these to choose the elevation to section, direction and where to place the section on the sheet.

Whoa! I tried it, it WORKS--IT" ALIVE! Thanx for that

 

[Richard Hed]

That's AWESOME Gordon! You're catching on! I'm glad you're sticking it out.

As Jason mentions, instead of assembling ALL the individual parts, create some sub-assemblies & then assemble those into your model. Please understand I've never ran Alibre, & can only comment on a "Workflow" I'm familiar with. I would typically create an assembly that would include the piston, wrist pin, connecting rod, bearing, & cap & assemble that sub-assembly into my "Top Level Assy.". When you get "Farther" down the road you'll understand this better. In the file I'm posting, it all looks like just a "few" parts right? Well, all the sub-assemblies are broken down & deatailed (This cuts down on my BOM showing a 'bazillion individual parts...

Yes, yes--that's the way to do it. Make several sub-assemblies with a few parts then if necessary build an assembly of sub-assemblys, then a super-assembly. That's when the object is very complicated. I only have gotten to subs then simple assembly of the subs.

 

[Richard Hed]

Although I don't use it much Alibre also has the "hide" option in assembly. Either right click the part on the screen or down the tree then click hide from the drop down list, you will need to do the same to bring it back but can only do that down the tree as it won't be on the screen to click

I have never used that 'hide' altho' I have seen it and presumed it to be something one just wanted to get rid of but not deleted. Never thot of using it that way. THanx.

 

[GreenTwin]

You can suppress things in Solidworks, which I guess is like hiding them.
You can suppress things like sections too, and toggle them on and off.

I hit a stumbling block one time when I turned a surface transparent, and then could not figure out how to undo that.
SW has a little trick where you can pick and then select several surfaces from a list.

Eventually you figure out all the tricks, or figure out enough tricks to be able to use the software.
You are off to a great start !!!

.

 

[Jasonb]

Careful there are subtle differences between Supress and Hide in Alibre and I expect SW is the same

If you supress an part in an Alibre's assembly it will not just remove the part from the screembut also all the assembly constraints relating to that part. So lets say you supress the crankcase to do some internal assembly then if you are not carful that crankshaft that was positioned relative to the case could move out of position. When you untick supress all will be active again - part and and associated constraints such as co-axial or coincident, etc

Hide retains all the assembly constraints but just gets the part "out of the way"

One other point for those assembling in Alibre, you usually constrain two items at a time, the first one clicked will usually stay in position and the second one move to it which is worth remembering if you have not tied either item down before trying to add constraints.

That then brings us on to Anchor, I like to position the first part which is often a crankcase or engine frame so one axis passes through the crankshaft ctr line and then anchor the part. That way you don't end up with your assembly suddenly ending up at some random angle and position.

 

[GreenTwin]

Careful there are subtle differences between Supress and Hide in Alibre and I expect SW is the same

If you supress an part in an Alibre's assembly it will not just remove the part from the screembut also all the assembly constraints relating to that part. So lets say you supress the crankcase to do some internal assembly then if you are not carful that crankshaft that was positioned relative to the case could move out of position. When you untick supress all will be active again - part and and associated constraints such as co-axial or coincident, etc

Hide retains all the assembly constraints but just gets the part "out of the way"

I will have to dig into that.
I have mainly used "supress" to hide the machining allowances that I add onto the model after it is complete, in order to turn it into a pattern.
So perhaps that is why I have gotten away with using supress without affecting the model.

Here is a SW tutorial.
There are so many options in SW.
Every time I watch one of these videos, I learn new things, but getting an overall grasp of how one thing affects another can be tricky, and I am still learning that.
The position in the tree is also critical, and you can drag things up and down the tree sometimes to fix things, and sometimes not.

 

[Jasonb]

Pat we are talking of Hide (and now supress) in the context of Assembly not individual part modelling.

 

[GreenTwin]

For the casting folks:
And before I forget, if you assign a material property to your model in SW, you can see the mass of it in whatever material, such as aluminum356 or gray iron.
Thus you can estimate how much metal to put into the crucible, if you are casting your parts.
Very useful feature.

.

 

[GreenTwin]

Pat we are talking of supress in the Assembly not individual part modelling.

Ok, I can't comment on that, since I don't recall ever doing that.

.

 

[Gordon]

One of the things that I am still trying to get straight is when I remove extrude something if it should be in + or - direction. So far it is kind of a guess. If it seems to do nothing I go back and right click on the extrusion in the tree view and edit so I can change the direction. I was having a problem with getting the part oriented in the right direction and I just discovered that the part snaps to the specified plane if you hit reset view. I am finding that it is handy that when you place your cursor over items in the tree they highlight so you can choose that item. All rather obvious once you see it but not so obvious to us newbies.

 

[Jasonb]

A lot will depend where you have sketched the shape you wish to "cut extrude" if it is on an surface then it tends to default to - so it cuts into that surface. if on a plane it will again default to - but that may not be the side of the plane you want to cut into so it needs to be changed in which case "reverse" is the quickest way to change the direction as you don't have to re enter the value. Hitting tab after any change will show it's effect rather than having to close the extrude dropdown.

It is also possible to name any of the features in the tree to make it easier when you go back to edit something, I only tend to do this for complex parts a sit's not worth it for a part that is only made up of a few features.

You can also right click the feature or sketch outline on the model and select edit rather than try to find it on the tree