Replacing 2 parts with 1 1

[Adrian2]

Dear Folks;

I have 2 lenses in a camera assembly which I want to replace with a single lens.

Could anyone share some suggestions about doing this. My main concern is replacing the 2 lenses with a single one without losing the position in space in the assembly.

The 2 lenses are both fixed in the assembly presently. Maintaining the same position is critical.

Best Regards

Adrian Dunevein

http://www.aaadrafting.com

 

[SBaugh]

If you try to replace both parts with one part you will get 2 of of the same single part at both locations. There is no way that I know of that you can do to get around this. You can replace one of the parts and delete the other. You might have to replace or repair the mates, once you have got the file in place.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If you are in the SW Forum Check out the FAQ section

To make the Best of Eng-Tips Forums FAQ731-376

 

[Heckler]

So correct me if I'm wrong. You're basically making a subassembly out of the two lenses and reinserting it into the next level assembly. I would set up some reference planes in the assembly that hold the critical position. It's a good practice to set critical positions with reference planes. Giving a plug for Pro/E they have a thing called skeleton part that allows all critical datum interfaces to be set within.

 

[CorBlimeyLimey]

Hmmmm .... I'm having trouble seeing how one lens can be in the same place as two. Are you able to post a picture to the web, either for showing here or viewing seperately?

My first thought would be to create planes in the camera assy, which are placed relative to the known postion of the 2 lenses & then create matching planes in the single lens. Then mate the planes in the assy to the planes in the single lens? Is that possible?



from (the City of) Barrie, Ontario.

What happens if you get scared half to death twice?

 

[Adrian2]

Dear Folks;

Thanks for the insight.

To clarify, I should point out that the single lens is a replacement for 2 lenses that were placed flat face to flat face. The single lens has exactly the same dimensions and shape as the combined 2 lenses.

Sounds silly I know, but I have to recreate the blasted things as a single part.

So far I have attempted to create a new part by part combine add command and this looks like it will work. But I am unfamiliar with part combines and the method of joining the 2 lenses together (part translation)is totally different from operations such as mating in an assembly.

I can also create a new subassembly consisting of the old 2 lenses, which is pretty easy. I had heard there was a way to turn an assembly into a part file, and was hoping someone might know how to do it. If I have to retain the the new assembly, it might mess up my bill of material structure.

I understand that when I insert the new part or new subassembly back into the top level assembly of all the optics, I am going to have to have some planes or reference points to get the part located in exactly the right spot. Trouble is , I cannot reference any planes or points to the old parts, because once they are deleted, my reference planes would have dangling references.

It should be possible to sort everything out but I still wonder if there is a preferred method for doing this as it cant be an uncommon occurence.

Best Regards

Adrian

 

[SBaugh]

Combine will not join two separate parts together. See Combine in the Help file. It's good for multiple body parts. You can subtract one body from another body. you can take 2 bodies and add them together to make a single solid-body.

To turn an assembly into a part is simple - File\Save As - Change the save as type to part.

Measure the parts at their location now. Offset the planes USING the Default planes at the assembly level. Then you can use those planes to mate with later. See faq559-871

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If you are in the SW Forum Check out the FAQ section

To make the Best of Eng-Tips Forums FAQ731-376

 

[Adrian2]

Thanks Scott;

You have likely saved me a lot of meddling about !

Adrian

 

[jhricm]

I have used combine before to take two parts and make them one. Just by inserting both parts into a part file and using combine to postion them and then adding or or subtracting other features. Is this the wrong thing to do?

 

[drawoh]

Adrian2,

Why are you combining two lenses into one?

Design issues like this are relevant. Design and documentation consideration ought to affect the way you create your model.

Most lenses have spherical surfaces, and are trivial to model in SolidWorks. Just do a rotation. If you have an optics textbook handy, it is easy to create a lens model based on diameter, thickness, index of refraction, wavelength and required focal length.

If your lens is custom, you need a drawing showing the dimensions, including the front and back spherical radii. If your lens is off the shelf, the manufacturer probably shows the radii in their catalogue, or they provide enough information that you can calculate the radii, either from optics equations or from geometry.

Most manufacturers of aspheric lenses will give you the coordinates required to profile the curved surface, so it is still fairly easy to make a rotatable sketch.

You need an accurate model of the lens to design or at least verify the functionality of your housing.

JHG

 

[Adrian2]

Dear Drawoh;

I did not create these models at all. All of the lenses were provided to me as iges files created by a contractor who did all his his work in PRO-E for a company that only uses solidworks.

The 2 lens combination was supposed to have been 1 all along, and yes it is trivial to model, but it should also be trivial to turn it into 1 part.

The only reasons I would like to have 1 part is that it makes my BOM more consistent and more importantly;
The customer wants me to do it that way !

Thanks for all your suggestions though, your input is greatly appreciated !

Adrian Dunevein

http://www.aaadrafting.com

 

[SBaugh]

CBL - you mentioned above:

Hmmmm .... I'm having trouble seeing how one lens can be in the same place as two. Are you able to post a picture to the web, either for showing here or viewing seperately?

See the below link and download the image files. That should help you undestand what I'm talking about. I assume you were talking to me.

http://www.scottjbaugh.com/Replace_Components.zip

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

If you are in the SW Forum Check out the FAQ section

To make the Best of Eng-Tips Forums FAQ731-376

 

[CorBlimeyLimey]

Hi Scott,
Actually, I was replying to Adrian2. I was having trouble understanding how he could be:-

replacing the 2 lenses with a single one without losing the position in space in the assembly.

How could one instance of a part be in the same place as two? His 2nd post clarified his situation for me, but thanks for the follow-up anyway.


from (the City of) Barrie, Ontario.

I tried sniffing Coke once, but the ice cubes got stuck in my nose

 

[drawoh]

Adrian2,

If you are trying to do as little work as possible, create an empty assembly, insert it into your camera, then drag the two lens parts into it. Open the assembly and fill in the BOM. When you make your drawings, just hide the interface lines.

If this ProE guy lacks the skill needed to model a biconvex lens, advise your boss never to deal with him again. I suggest that you check the rest of your model very carefully. Someone that dumb probably did something else stupid. With IGES you can verify that everything is correctly to scale, if nothing else.

Consider the possibilty that he is not an idiot. If the rest of the model is competently constructed, it is likely that there was a good reason to model two plano-convex lenses back to back. You, your boss and your customer might need to know what this is.

My comments above are still valid. Either...

a.) ...it is a custom lens for which you need accurate scale drawings,

b.) ...or it is a standard lens with a manufacturer and part number which will succumb to a Google search.

If you are not creating accurate scale models, SolidWorks is a waste of time.

JHG

 

[Heckler]

Also, if this is a critical part of the design their should be a source control drawing and procument specification to go along with the model. In which, all critical interfaces should be defined. Anything less and it's a crap shoot. This guy works for you based on the specification document so he should provide you the data as you require it. The trouble with contractors these days is they want the $$$$$ but don't want to deliver the goods. I spend a good portion of my day chasing down flakey subcontractors.

 

[Adrian2]

Dear Heckler;


Ouch !!!!

As a contractor I will have to remember to steer clear of you as I'm dragging my next sack of money to the bank !

Have a good weekend anyway


Adrian

 

[Heckler]

Hey Adrian,

Nice website! I'm sure you're the exception to my expereinces. I've been on both sides of the fence an independent contractor and now an employee. I found it helpful to my getting repeat business to go beyond expectations. How much work do you currently have going through AAA?

Vince

 

[Adrian2]

Dear Vince;

AAA Drafting is my main source of income and has been so for the last 8 years. All of my business is through repeat customers.

One of the ways I try to go beyond expectations is by relying on resources such as this forum. Despite my 18 years in mechanical drafting, I come here and still learn new ways of doing things.

The lens issue is not really as important as knowing that there are many ways you could go about doing it. Sometimes when you are stuck, knowing 3 ways to get out of trouble instead of just 1, makes all the difference.

While I was jabbering away in this forum yesterday, my helper joined the two imported solids into 1 by surface knitting them. Now we have a nice drawing for the assemblers with all the ordering information clearly presented in the bill of material.

everyone lived happily ever after

untill the next impossible deadline !

Best Regards

Adrian

 

[jhricm]

Adrian,

I have used combine before to take two parts and make them one. Just by inserting both parts into a part file and using combine to postion them and then adding or or subtracting other features.

In one instance it was decided that two plastic parts could be molded together as one part. I used combine instead of re-drawing them. I could still then open up and change each part seperatly or add to and subtract from the cobined part.

Is this the wrong thing to do?

Thanks
Jim