I had a quick and probably very easy question to answer. I have man different size counter bores and want to use leaders to point out th same size counterbores from a single dimension. I've tried everythin in the help folder and nothing is working for me. I can do it wit anotations but not with dimensions. Any help would be greatl appriaciated Thank Ale
I think I understand what you are after. I've been in the same boat before. You just need a good way to clarify which holes are grouped with a particular size.
The solution I use is to use a hole table. This automatically puts tags on each hole, and groups them by letter. For example, you may have holes A1 thru A12, B1 thru B26, and C1 thru C8. This would be 46 holes total, but 3 different sizes distinguished by the letter. SW will automatically determine "like" holes and group them.
Now there are a few of options you can do here depending on how you want your hole tables setup:
You could have the hole table call out nothing but the locations and grouping (A's, B's, C's), and use a hole callout (or dimensions) on the holes themselves.
You could have the hole table callout the hole sizes by grouping them together (A's, B's, C's), then use dimensions in the view for locations.
Or you could use the hole table entirely to call out the hole sizes and locations by grouping.
Hole tables work pretty good. They help keep the clutter down as well. I use them a lot...
Hole tables are indeed nice, but I run into this problem too when calling out two or three corners or fillets of the same radius. Has anybody blundered into a solution, yet? (Not to belittle the more skilled people out there...blundering's my usual method).
You add a note, and instead of typing, click the dim. The note is tied to the dim and you can use multiple leaders.....
Personally, I think this workaround sucks as besides the fact that you lose the ability to make changes from the drawing (if you do that), but it does not allow for use with tolerances. You can type +/-.005 after the dim is inserted, but try dealing with a bilateral....I wish they would include a multijog capability with the dim. They could make it that the dim is inserted as normal, and any additional leader should you decide to add any are reference only and are not tied to dimension. They can even give that as a warning in a message box when you go to use the dimensional multijog (with an obvious checkbox not to display anymore as not to annoy ya..)
I commonly just draw a single leader that is a bit longer than normal, and type the text for the dimension. Then I add additional leaders to the other simlar objects and end those leaders at the first leader (just hitting return at the text prompt will leave it without text).
As far as I remember from my drafting book, it is not acceptable to dimension multiple radiuses with multiple leaders comming off a single dimension. Not sure why, but I think that is within the drafting standards. Someone correct me if I am wrong please.
I usually just label one and type (TYP. # PLACES) after the dimension if it is obvious which radiuses are the same.
firstname.lastname@example.org (woodcutter) wrote in news:ELWdnRSQf_Z8Z97eRVn email@example.com:
Most help files suck, unless you know what you're looking for, in which case you probably don't need to look for it.
folder and nothing is working for me. I can do it with
Having read some of the responses to your queary, I have this to add.
I too have had the situation where a cluster of holes becomes difficult to distinguish and a single dimension with a note like "TYP" or "4X" won't do.
I dimension one hole normally. Then dimension the other (of same size) holes and place the dimension near the first and erase all text and values from the dimension, (there is a warning message) leaving just a leader. I drag the leader to the first dimension (it alligns quite redilly) and voi- la. Now to reposition them, I select the original dimension and the extras together and they all move and stretch accordingly.
Yes it does deviate from convention. However, many shops develope their own convention, adapting from the ANSI, ISO or such as a starting point.
It is associative to the first hole only. (that's a given) Dimensions to holes created in a sketch (with a circle) retain associativity and the values can be restored. It would be easier to just re-dimension. Holes created with "Hole Wizard" tend to dissasociate in most cases. (have you ever changed threaded hole to a thru hole?
Merely a mention to say that it is not a complete workaround as try adding a associative bilateral tolerance to that dimension or chamfer...I didn't say there was a better way, now did I? I know that drawing standards indicate that while it is not a correct usage to have multiple leaders, it is very commonly used as a means for a cleaner print where you might have several varying sizes of radii, corner fillets, chamfers and undercuts in the same general tight location....Doesn't mean it's right to use, but sometimes it saves additional detail views and perhaps additional sheets. I do however agree that there really is no need for it's usage on hole callouts as hole tables handle them quite nicely. Now chill - No need to get your panties in a bunch over it, "smart guy"....