assembly driven part features?

[Jasonx10]

Im currently working with SW2007. I'm designing 2 fixtures to check length tolerances on this wire harness. One fixture will check the mean part print dimensions, one will check the min. part print dimensions. I have one big bass plate and about 15 different riser brackets with clip-blocks that that various connectors on the wire harness plug into.

Since i have one mean-size fixture and one min-size fixture i have drawn out the part itself to min and mean size and have used the mean configuration of that wiring harness as a basis for the riser bracket hole locations in my base plate. All my assembly mates move relative to the wiring harness. Is there any way i can base the location of those mounting holes in the bass on the position of my wiring harness and brackets in the assembly? In other words - if i move one of my brackets in my assembly i want the mounting holes in the bass-plate part file to change and update accordingly?

I know i can add cuts to an assembly file, but I guess im trying to use assembly mates as a basis for the location of holes on an individual part in that assembly.

Hopefully this makes sense. Thanks!

 

[SBaugh]

You would have to in-context your part file to something in the assembly. You cannot control a part at the assembly level without first in-contexting the part.

See the help for understanding of Top-down design.

You would have to edit the part at the assembly level and make the hole using something of the assembly or other parts to control its location, so if you do move something in the assembly the hole will follow.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[ShaggyPE]

To add to what Scott is saying. Edit the sketch of the mounting holes in the baseplate in the context of the assembly. Next, delete (or make driven) the dimensions that are positioning those holes. Now make those sketch circles (if you are not using hole wizard) or sketch points (if you are using hole wizard... recommended) concentric to the holes in your riser brackets.

The one thing you will need to make sure of is that in your assembly, you are not mating your riser brackets concentric to the holes in the base plate. Because at this point you will have a circular reference.

-Dustin
Professional Engineer
Certified SolidWorks Professional

 

[Jasonx10]

I was able to edit the base plate in the assembly. I just put 15-20 tapped holes in and was able to snap them central to the mtg. holes of the brackets, but is their a way to set relations in the assembly (my goal is to get these to update when i switch to an alternate config)? I must be missing something here.

The insight i gleaned from sw help was to in-context something i can simply right-click the desired part and edit it within the assembly.

In order to set relations between those bracket mtg. holes and the base holes do i have to <i>create</i> a part within that assembly based on an assembly sketch?

Thanks very much

Jay Warnke

 

[MadMango]

You wouldn't have to create a whole part, the new features you are adding to the edited part in the assembly will be in-context. I guess it also depends on what your configurations are actually changing as well.

"Art without engineering is dreaming; Engineering without art is calculating."

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[CorBlimeyLimey]

When dealing with configs, it is often better to use Feature Driven Patterns (from the driving config) when creating matching holes. That way when a config with a different hole quantity pattern is active, the matching holes will update. If individual matching holes are placed to the centres of an active config, the matching hole quantity will not update when the config is changed.

 

[fixturefanetic]

The great thing about SW2007 is you can get automatic relations. When adding your holes in context, swirl your cursor over the hole you want to be concentric with. Your center point will show up. Grab the center to draw your circle and drag it until it is coradial. If you then go to your part and add a dimension to the radius you will find that the sketch is totally defined. When you move your hole in the mating part, it will move both holes. When using cleco's to fasten large assemblies prior to welding, this function comes in very handy.

Fixturefanetic

 

[Jasonx10]

Hrmmm. No go yet. I uploaded a picture of this. Maybe it will make a bit more sense.

Right now the brackets that you see are driven to their positions based on lengths of a wire harness that they mate to in the assembly. I have mated the base plate with distances from its faces to the central planes on the wire harness. I also mated all the riser brackets parallel to the bass plate surface.

The red circles are some tapped holes that i while in the assembly cut into the base plate part. While in my hole wizard i was able to drag and drop the points of the holes concentric to the centers of the thru holes on the corresponding brackets, but the points remained blue - undefined.

When i switch to my short-length wire harness config, all the brackets move with the wire harness - the base plate stays in position relative to the distance mates i made between the base plate and the wire harness planes, but the holes i cut in to my part do not move and stay concentric to the bracket holes.

Sorry for all the questions! Ill stop bugging you guys after this. Thanks

 

[CorBlimeyLimey]

Do you have the Automatic Relations tool activated?

Are you pre-selecting (clicking on) the face before activating the Hole Wizard?

 

[Jasonx10]

yes automatic relations are on and also yes on the pre-selecting the face.

 

[CorBlimeyLimey]

Are the brackets fully constrained?

 

[ShaggyPE]

I had to squint to see your feature tree in the image you posted, but I was able to notice that your hole feature does not have the -> symbol after it. The -> symbol indicates that the feature is in-context. You also mentioned that the sketches were not stating that they were fully defined. If you are using hole wizard, only one relation will fully define them (therefore my guess is that there are no sketch relations holding them to the brakcet). While in the sketch, hit the icon that looks like an upside down T with glasses. This will display the sketch relations. You should see a bunch of coincidents or concentrics that all have the -> after them. If you don't, then the automatic relations did not occur and you will need to do them manually.

-Dustin
Professional Engineer
Certified SolidWorks Professional

 

[fixturefanetic]

After you have placed your holes using the hole wizard, you may need to edit the 3d sketch in context and drag the hole location astrik until it grabs the automatic relation.

Fixturefanetic

 

[ShaggyPE]

If you select the face prior to selecting the hole wizard icon, you won't have a 3D sketch. The 2D sketch plane will be on the selected face.

-Dustin
Professional Engineer
Certified SolidWorks Professional

 

[SBaugh]

Do you have the "Large Assembly Mode" active under Tools? That will keep you from doing certain functions inside of an assembly.

Also, you need to learn how to use the Command Manager... its so much easier to use IMO and it saves on a A LOT of real estate for the graphics area.

Attached is my working area in an assembly.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376