Question: Scaling Bodies or Sketches

I have a part that consists of many bodies. I need to scale the location of many (not all) of the bodies. I don't want the bodies themselves to scale, only the location. Is there a way to scale the LOCATION of SOME of the bodies without actually scaling the bodies themselves?

As an alternative, I think I know of another way I could achieve what I want with body patterns, but only if there is a parametric way to scale a sketch. Anyone know how this can be done?

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Seth Renigar
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2D sketches can be scaled using the "Modify Sketch" tool as long as they have no external references

Seth Renigar wrote:

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Insert mold, huh? I'll think about it.............


Reply to
John Kreutzberger

What about the Move/Copy body feature?

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Unfortunately, my sketch does have external references. Besides, this is not a parametric solution. Once the tool is used and closed, you can't change it or control the scaling in any other manner.

Here is what I have in a nutshell (simplified version). Let's say I have a plate with many holes in it. The locations are defined in context therefore they are currently fully defined. Now, after the hole feature is defined, I need to scale the locations, and only the locations of these holes.

What I am currently doing works, but is very time consuming. I am creating a reference sketch, putting points on the current hole centers, and adding reference dimensions to each of these points. The sketch also has a converted edge of one of the hole diameters with a reference dimension pointing to it as well. After that, I delete the original holes using delete face. Then I recreate a holes with a hole feature putting the points in approx. the same location as they were. I dimension them using the same dimensioning techniques as I did with the reference sketch. Finally I add Equations to each of these location dimensions referencing the dimensions in the reference sketch and adding a scaling factor to it. I can keep the same hole diameter by tying an equation to the diameter dimension in the reference sketch. So what I end up with is a series of holes with the locations scaled from the previous original holes, but the size remaining the same. If the locations were to change in context, the scaling would also change appropriately. But when you have got 50-100 holes to do, this gets intense.

There has got to be a better way! What am I missing?!?!?

Reply to
Seth Renigar

Actually no. However the insert mold situation could use a similar technique.

See my response to horatio.hornblower for a simplified scenario of what I have.

The reason I originally asked about scaling bodies is that I thought I could create bodies from my holes, and scale the body locations to create new hole locations. I was not thinking correctly. I forgot that scaling would scale location as well as size.

Reply to
Seth Renigar


If I understand your description correctly, I think there's a way to simplify the process.

This would be to create a sketch as a collection of location points to be used in developing a Sketch Driven Pattern.

When the pattern is defined you can use a single pre-existing Hole Feature (Cut-Extrude, Simple Hole or Hole Wizard type) to automatically populate it with the copied hole axes centered on the point locations.

If all 50-100 holes are not the same, then you'd need a separate sketch for each Sketch Driven Pattern definition.

Just as in the "reference" sketch you described, there would need to be an entity to use in keeping track of the scaling. There's no need to use any in-context conversion of a hole diameter - a construction circle dimensioned to be a starting unit of "1" (inch or mm, etc.) will do.

After the Sketch Driven Pattern is defined, simply use the Tools/Sketch Tools/Modify function to execute a scale change. The original reference circle of "1" unit will become .5, if the scale is made to be one half.

After the first scaling, the reference circle will report a dimension of ".5" unit and, if the sketch is scaled again, changing it back to full size ("1" unit) would of course require a scale factor of 2 and setting it to be 1/4 of the original "1" unit would require a scale factor of 1/2.

Keep in mind that, in order to scale a sketch, there can be no external references. This means that it may be necessary to fully dimension the point locations (instead of using relations) and to delete the X and Y dimensions which locate the entire pattern of points. After the scaling is applied, the X, Y dimensions to the origin of the point patttern can be reapplied.

Hope this helps...

Per O. Hoel

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Anyone got a solution to my problem below?

Reply to
Seth Renigar

Create construction solid body with holes in it (if you want, holes parametrically linked to outside body). Scale this construction body. Don't care if hole diamaters change, you are just using it to locate the holes on the final body of your part. On your final body, all holes have diameters dimmed as you wihs so they don't dhange, and are concentric to the holes in the construction body. Use reference dims to get dims into drawing.

Feature tree looks like this: construction body construction body holes construction body scale Main (final) body - do not merge with construction body Main (final) body holes (located with relations to sacrificial body holes) - do not merge with construction body Delete body (construction body)


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sounds like you could use a design table...

"Seth Renigar" wrote in message news:mTdxf.11717$

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For some reason, your post did not come through to my news reader. I saw it on Google groups, so I am replying from there.

Anyway, thanks for the reply. I am not sure that I follow exactly though.

I have to create the original holes in-context. There is no parametric way of getting around this that I know of.

I do not like to use the Tools/Modify function anyway. Once used, you can not control it any further.


POH wrote:

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Ed, YOU DA MAN! This worked perfectly. Now to make a scaling adjustment, I all I have to do is change the scale of the construction body. And, if any holes change locations from the original in-context feature, they automagicly scale in location properly.

Here is the final outcome: (the part in question has a base part inserted as the first feature)

  1. Insert second base part body from the same base part as the original base part (now contains 2 identicle bodies)
  2. Scale second base part body as needed
  3. Create reference sketch, with driven dimension, defining only the hole diameter from first base part body (will be used later in an equation)
  4. Delete the existing holes from the first base part body
  5. Insert new holes in the first base part body using the scaled second base part body for locations only
  6. Delete second base part body
  7. Create an equation driving the hole diameter only, from the reference sketch

What I end up with is the original first body with only the hole locations scaled. And, if anything were to change in the assembly that has the in-context reference, including hole size or location, the part would update correctly.

This is definately one to remember.

Thanks, Seth wrote:

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