ASSEMBLY INSTANCES 1

[CADGemini]

Hey Everyone,

I was wondering if there is a way to change the instance of a component in an assembly. Let's say I have a plate with 20 holes in it. Each of those holes have the same screw assembled into it. Now if the plate changes and we lose the first ten holes then I also have to delete the first ten screws. Now my screws have an instance number from 11-20. Is there a way to update the instance of each of those screws? If there is a work-around for this I would love to hear it.



LIFE IS WHAT YOU MAKE OF IT!!

 

[aamoroso]

Create a Second Configuration of the plate. When you insert the fastener in the assy mate the first instance to the first hole created in the plate. When you change configs of the plate, the hole pattern will change, so will the Feature Driven Component Pattern in your assy. You should create a second configuration in your assy for this type of work.

 

[CorBlimeyLimey]

jkintest
To expand on aamoroso's post ... the holes in the plate should be a Feature Pattern of one hole which must always remain in all the configurations. One screw should be mated in the original hole & a Component Pattern of that screw should be made using the Feature Pattern of the holes.
Then when you change the parts Feature Pattern of holes (by whatever means), the assemblies Component Pattern of screws will be updated to suit.

from (the City of) Barrie, Ontario.

If you choke a smurf, what color does it turn?

 

[CADGemini]

Thank you both for your suggestions. That helps out alot. I have been trying to gear our drafting department to using hole wizard and this is just the info i need to convince them it is the best possible way.

 

[CorBlimeyLimey]

If you use the Hole Wizard to create the pattern of holes (ie. by placing multiple points) you will not have an "original" hole in which to mate the first screw, nor will you have a Feature Pattern to use in the Component Pattern.
By all means use the Hole Wizard, but only to create the first hole, then pattern that hole using one of the Feature Pattern options (Linear, Sketch driven, etc) so that it can be controlled by a DT or Equations for the part configurations & in turn be used to pattern the screws in the assembly configurations.

from (the City of) Barrie, Ontario.

If you choke a smurf, what color does it turn?

 

[ShaggyPE]

To add to CorBlimeyLimey's post, the first point you create within hole wizard is the "original" hole. This point is where the revolve cut will be made. If you mate to this hole, then add more points in the hole wizard sketch, the component pattern will update correctly. I use this method all the time.

But for your purposes, the single hole and feature pattern will give you more control when using a design table. You will be able to control the number of instances and spacing much easier.

 

[CADGemini]

CorBlimeyLimey,

I have found that is not the best method of using hole wizard. For one if you use the method you are adding an extra feature to your tree. if you contain the hole pattern in the hole wizard it make things much easier to mate screws and such. All that we do here is fully define the mates of the screw to the first hole of the hole wizard. Then we use INSERT/COMPONENT PATTERN.../FEATURE DRIVEN... Then select the hole pattern feature to drive the rest of the screws to their locations. All of the screws are now fully defined.

THERE ARE SO MANY WAYS TO SCREW IN A LIGHT BULB. (figure of speech)

 

[CorBlimeyLimey]

I have to admit that I did not realize that a series of holes, created using the Hole Wizard, could be selected as a Feature Pattern for subsequent component mating. Thats handy to know ... Thanks

However, uing this method does not lend itself to configuration control using a DT or Equation, as the qty of holes is not available for selection. The quantity has to be manipulated at the Holes sketch level, by adding or deleting points. I prefer to modify the part size & have the hole pattern automatically conform to a predetermined set of rules based on that.

"To each his own". If the way you do things suits your product & keeps the bosses happy, then thats great. I'm happy because I learned something new.

from (the City of) Barrie, Ontario.

If you choke a smurf, what color does it turn?

 

[CADGemini]

Your welcome CorBlimeyLimey. I am still trying to learn how to use design tables and equations, but I do see your point of having more control over the holes. I'm glad you were able to learn something new from my post even though it is not of much use to you. Well if you need any more useless information I will always be happy to help. LOL!

 

[SBaugh]

http://www.solidprofessor.com/Newsletter/may2004/sptip1.html

Try looking into this. I know you can get a CD that has a 3 Day Trial. It's very good not only in content, but because I was looking through the basic information and even though I know the basics, for some reason I was compelled to watch it.

Regards,


Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[CADGemini]

Thanks Scott,

I have been to that website before but must have overlooked the design table tutorial. Do you know of any good websites to get Photoworks textures? I've been to a few but haven't found any spectacular websites that are worth saving to my favorites. Just curious.

Thanks again...

 

[SBaugh]

There are 2 of them here that I listed. There are links from there that I'm sure will probably help.

faq559-520

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376