Add tolerance in part with hole wizard 1

[VELCROW]

I'm creating several parts that have dowel pin holes, and I am using Hole Wizard to get the automatic callouts. I create the hole with the correct dimension, and have the correct tolerance right in front of me, but there is no place to enter the tolerance into the dimension. I can put it in the hole profile sketch, but it does not show up in the drawing. Right now I just wait until I create the drawing (days later) and then have to go back and look up the tolerances again.

I could just use extrusion cut, but I lose the automatic callout (depth, quantity). Any suggestions?

Thanks,

Steve

 

[CorBlimeyLimey]

If you use the Import > Model Items method, the manager has an option to select the Hole Wizard Profiles dimensions. When that option is used, the tolerance is displayed.

 

[VELCROW]

Thanks for the quick response.

Did you mean Insert>Model Items in the drawing file?

That does indeed allow me to display the tolerance I entered into the part, but I lose the depth and quantity callouts. Sorry to be picky, but no real improvement from the Extruded Cut method.

 

[CorBlimeyLimey]

Sorry, yes I did mean Insert > Model Items.

If you want to use the Hole Callout with tolerance shown, you have to click on the callout and add it in the manager that appears. That only works for the dia, not the depth.

Hopefully SW2010 has improved this.

 

[Gupta65]

Double click the hole feature and then click on depth dimension. Then you can add the tolerance.

Deepak Gupta
SW2009 SP3.0
SW2007 SP5.0
MathCAD 14.0

 

[VELCROW]

Deepak,

I double clicked on the hole feature in the graphics window, then double clicked on the diameter dimension (the one I want the tolerance on). I was able to add tolerances, which show up in the part. But when I make the drawing, there are no tolerances. If I turn on the tolerances in the drawing dimension, they are .000, not the .005 I entered in the part.

 

[Gupta65]

Velcrow, I'm able to do that here with SW07. Check attached pic. If you looking for this, I can put up a sample file. Also check for dimension unit decimal places.

Deepak Gupta
SW2009 SP3.0
SW2007 SP5.0
MathCAD 14.0

 

[ShaggyPE]

My understanding is that Velcrow wants all of the tolerance information in the hole callout itself.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[VELCROW]

Ideally, yes. I'd like to have it look like all the other callouts, with just a leader pointing to the circular hole.

 

[designer22]

Hi VELCROW,

Are you looking for something like this?
You can insert hole call out from the Annotation Tab.

I hope this helps.

 

[VELCROW]

designer22,

That is the end result I am looking for. As I mentioned above, I am using Hole Wizard to get the automatic callouts you showed, but Hole Wizard does not let me enter tolerances into the part, as far as I can tell. I must wait until I make the drawing, which could be days later, or I must use extruded cuts which does not give the full automatic callouts.

If you put those tolerances into the part, and not the drawing, please let me know how you did it.

Thanks,

Steve

 

[designer22]

The steps are same as Deepak explained above.

Create the hole using Hole Wizard.
Edit and Modify the sketch created by the Hole Feature.
Add the proper tolerance to the Sketch Dimensions.

Please see the attached picture.

Thanks

 

[VELCROW]

designer22,

I think I am not being clear, so let me start from the beginning. The attachment shows what I want as an end result - a top view, not a section, with a callout of diameter, diameter tolerance, and depth.

I want to put all the relevant information in the part so when I make the drawing later I do not have to go back and look up tolerances.

I want to use the Hole Wizard, because I can then use the Annotations to pop up exactly what I want in the Drawing.

BUT, if I enter the tolerances on the Hole Wizard sketch as you suggest, they don't show up in the drawing callout. I turn on the tolerances in the drawing, but they come up zero, even though I have a value in the part sketch. (I got the tolerances in my attachment by adding them in the drawing.)

I put the tolerances in the part. Can you tell me how to show them in the top view callout?

 

[CorBlimeyLimey]

After placing the HW hole(s), edit the seed profile sketch dimensions to include the tolerances required. When the views have been placed in the drawing, use the manual Hole Callout tool to place the callouts.

For some mysterious reason, the Insert > Model Items hole callout does not include the tolerances.

 

[VELCROW]

I think I figured it out.

Insert>Model Items, with the Hole Callout button (lower right of the Dimensions section).
I get the diameter and depth, but no tolerance. When I click on the dimension, I can add the tolerance, but it comes out zeros. I can make it anything I want, independent of the part tolerance.

Insert>Model Items, with the Hole Wizard Profile button (lower left of the Dimensions section).
I get the diameter and the correct tolerance, but no automatic depth (no way to include depth parametrically at all, AFAIK) and no radial leader.

All the pieces I want are available, just not at the same time

But it seems like a bug, that the callout tolerance is not connected to the part tolerance.

 

[CorBlimeyLimey]

VELCROW ... read my post above yours. Placing the Hole Callout manually will include the tolerances from the part model.

 

[VELCROW]

Wow! That does it exactly. I never knew that manual hole callout was there, I always used the Insert>Model Items, which was often flaky for hole callouts. The manual method makes this a whole lot easier.

Thanks!