Hole Pattern Dimensions in Drawing

[ssmithdigilab]

When you create a pattern in a part, the pattern feature only gives you the option to define the spacing distance between features. Then in the drawing, the model dimension that shows up is the spacing dimension. I would like to have each hole dimensioned from the end of the part to minimize tolerance stack-up.

Is there a way to change the model dimension(s) of the pattern so that each hole is dimensioned from the same location on the part? I prefer to show model dimensions in my drawings rather than creating them, but it seems that I don't have that option here.

I think I remember being able to change this in Pro/E, but it has been a while since I've used Pro/E, so I'm not sure.

 

[CorBlimeyLimey]

The only way I know of is to add the dimensions in the feature sketch.

 

[Jwouters]

What about a hole-table?

 

[ssmithdigilab]

CorBlimey,

I assume you mean creating all of the instances in one feature instead of patterning? The only problem with that is it makes it tough to add fasteners to the assembly when you can't follow the pattern.

 

[mjcole]

Pardon caps I'm not lazy but didn't want to retype.

YOU CAN MAKE A SKETCH OF POINTS YOU WANT IN THE PATTERN AND DO A SKETCH DRIVEN PATTERN.

This will allow you to use Sketch pattern to get a good 2 directional pattern. and add reference dims.
This will create a pattern similar to pro/e's table pattern.

If you create a sketch pattern you can delete the relation and use fully define sketch with ordinate dims to get each dimension called out as a driving dim or keep the pattern relation and use the Ordinate as ref dims.

What CBL is suggesting is to do linear pattern using the offset dimensions from the hole placement sketch to do the pattern which as a Pro/E user you know used to be a requirement for patterns before they Direction Pattern was created. That may give you the dimensions in the pattern instances but I know that the Sketch Driven does. I'll try to do and post an example in 2009 and 2010 formats.

Michael

 

[CorBlimeyLimey]

ssmithdigilab ... If you use the Hole Wizard, the sketch points can be dimensioned individually but from a common datum. The HW set of holes, although not shown as a pattern, can be used/selected as such when placing fasteners.

 

[drawoh]

ssmithdigilab,

Do you absolutely have to display model dimensions on your drawing?

Apply reference dimensions. You can set these up any way you darn well please, while you model your features any way you darn well please.

JHG

 

[ssmithdigilab]

I don't absolutely have to display model dimensions. I simply prefer to. I feel that it is better practice to do this and it also creates a stronger relationship between the drawing and model. If you want to edit a dimension you can simply edit it in the drawing and it updates the model.

Creating dimensions in a model and then recreating those dimensions (or creating other dimensions) in the drawing seems redundant. Not to mention creating dimensions in the drawing allows for accidental over dimensioning and other mistakes.

I see a lot of older drawings here that have dimensions created in the drawing and they have somehow become detached from the features they were dimensioning. These dimensions are usually grey and have an incorrect value. That wouldn't have happened, had the person shown the model dimensions.

 

[EEnd]

I think the feature that you remember from ProE was a table driven pattern. I do agree that SolidWorks’ feature pattern is not amenable to supporting the design intent of locating all of the features relative to a common datum and its impact on tolerance stackup.

Eric

 

[ssmithdigilab]

Yeah, it was definitely the pattern table that I was referring to. It's been a while since I've used Pro/E, so the terminology is fading.

If you can indeed pattern fasteners to the hole wizard set of holes (as mentioned by CBL), then I will definitely just create them that way. I had previously been creating the holes using the hole wizard, anyways, and inserting the fasteners one by one. I'll have to try to patterning the fasteners the next time it comes up.

 

[CorBlimeyLimey]

When using the HW holes as a pattern, place the first fastener in the seed hole (see note below), and then pattern (separate feature) that fastener by selecting the HW feature (or one of the holes in the set).

NOTE: When creating the pattern, any hole can be selected as the 'virtual' seed hole, but I prefer to use the 'real' one.

 

[ssmithdigilab]

Just tested that out. It works great! Thanks a lot for the help, CBL, et. all.

Wish I had this information months ago. I've been wasting my time inserting fasteners one at a time.

 

[CorBlimeyLimey]

ssmithdigilab ... Are you aware of the other methods of mating fasteners?

http://help.solidworks.com/2010/English/solidworks/sldworks/assem_1/types_of_smartmates.htm