-
Foreshorten Linear Dimenions
Create it in the regular view, then CTRL+drag it over to the detail view. It is explained in the Solidworks help file labeled "Arrows Options".
Setting the foreshortened arrow type is set by going to Tools>Options...>Document Properties>Detailing>Arrows>Foreshortened diameter.-
Foreshorten Linear Dimenions
Thank you for the response but I have done all the things you suggested prior to posting on the forums. It is my understanding this only works for Diameter dimension either linear or in the standard dimenison style. However I am trying to utilize it in a means for a linear dimenion that is not a Diameter.
I am trying to attach a file to show just an example of what we are trying to accomplish. The 1.77 dimension in Detail A is the dimenions we are trying to foreshorten.
The detail was created then the 1.77 dimenions was CTRL+dragged into the Detail View as you see in the image.
Any suggestions? -
-
-
Foreshorten Linear Dimenions
If ya'll can figure it out let me know. I have tried to create a foreshortened dimension in a Detail view which comes from a Section view. I have tried the drag and drop from the standard view as well as from the section view. I have tried it using Ctrl-drag and Shift-drag....neither works. I even tried to fake one using a leader, only problem is I can't get rid of the text box. I am on the verge of violence!!! I thought 2008 was the cure-all.
-
Foreshorten Linear Dimenions
The best I have been able to achieve is to create the dimension and hide one extension line and one side of the dimension line - this by right clicking on it and selecting to hide it.
I have put an enhancement request on this. Maybe it'll go through if it gets some more votes.-
Foreshorten Linear Dimenions
I'll give you my vote for this one!! Can't get foreshortened dims to work on Diameters or lengths. Best work around I have is to use points to attach dimensions to such that there is only an extention line on one side and then direct a note to another point on the dimension line with a space in the note box to get rid of the box.
RUBBISH!!!
I also assume that foreshortening is something that only is supposed to work with model Items. As I do not always use model items could your ER also ask for foreshortened dims to work on standard dims too.
Thanks
DaveP -
-
-
-
Foreshorten Linear Dimenions
Double arrow foreshortening of simple linear dims is not provided for in the ASME or ISO standards because it does not provide enough information for the viewer to know where the foreshortening ends.Bradley Townsend wrote:
Is there any possible way to "foreshorten" a linear dimension in so that is shows the "double arrows" at one end of the dimension line in a detail views?
If you wish to show a dim that connects to a point off the part, the only way in the standards is to use ord (because the 0 is at a known location), though even that is not explicitly mentioned.
-
Foreshorten Linear Dimenions
Matt & Others,
Although foreshortening of linear dimension in broken and/or detail views is not identified in ASME or ISO, it is still a widely used and understood practice in the various industries.
I am not saying I agree with the practice but I believe it is a result of taking liberty with "Foreshortened Radii", 1.8.2.2, ASME Y14.5.
The standard identifies radii as be foreshortened via a jagged break in the radial dimension leader. Elaborated in the standard are additional provisions allowing the foreshortening of the linear dimensions that locate the radii's center.
I guess one's assumption is that if linear dimensions are foreshortened in this particular case, then all linear dimensions are fair game.
-
Foreshorten Linear Dimenions
I've not found this to be the case. There is no way to presume the other end of the dim if you don't show the other end. You may be able to make use of baselines (similar to how Ords are used), but this will have to be explicitly stated somewhere on the print. Even this possible workaround still requires a view of the other end somewhere on the print.Although foreshortening of linear dimension in broken and/or detail views is not identified in ASME or ISO, it is still a widely used and understood practice in the various industries.
Foreshortening of radii requires no such detail of the other end, which is why foreshortening is only applied to radii/diameters. Note, there are actually several ways to foreshorten radii. No ways to do so for standard linears. This isn't accidental.
-
Foreshorten Linear Dimenions
Matt,
Just a couple of final points (I think we beat this one to death!):
=> Even though "you have not found this to be the case", I guess we can agree to disagree.
=> I agree with your statement about the starting point of the dimension needing to be shown and/or identified.
=> Lastly, I do not agree with the example given by Bradley Townsend because, IMHO, it does not make any sense/no value.
However, I do agree with David Plowman's example for diameter. The funny thing is, "foreshortened diameters" work just fine for me. In the case of diameters, there is only one solution for the location of the opposite dimension arrow.
-
Foreshorten Linear Dimenions
Bradley,
Can you insert a vertical break in a detail view in SW 2008? I running an old version so I cannot try it. It won't give you the double arrowhead, but the break lines should convey the meaning.
KK-
Foreshorten Linear Dimenions
Here is a work-around if the zigzag is acceptable. You can sketch an arc in the detail view. Add a radiius dimension and a dimension from your edge to the arc centerpoint. You then make the radius dimension a foreshortened dimesnion. You can put the arc on a hidden layer, hide the radius dimension and hide the appropriate dimension and witness lines. This was done in 2009. I could not get the double arrows even though I have it set in the document options.-
Foreshorten Linear Dimenions
Just been having a mess around with this, nice and fresh after the weekend and I can get foreshortened dimensions to work but not in all instances.
The foreshorten function only seems to work if the dimension is made as a diameter dimension. I draw a lot of models as revolves and for some reason not all my diameters are seen by Solidworks as a diameter even though I draw them about a centreline. I'm sure I've seen a function somewhere to set a dimension as a diameter dimension but can't find it now I need it. Just putting a diameter symbol in front of it doesn't seem to be good enough.
A Workaround appears to be to extrude a cylinder prior to drawing your revolve to ensure that the dimensions are seen as diameters but surely there must be a proper way of doing this.
To summarize, I modelled a cylinder as a revolve and it did not work, I modelled a cylinder as an extrusion and then added a revolve and it did work.
DaveP
-
Foreshorten Linear Dimenions
I actually created symbols on the GTOL file for this. (RH , LH, Up and Down arrows). They work in most instances, unless you have to add notes to the dimensional values. The it can be difficut to get the arrows to line up correctly.
It works, but I'd much rather have the real thing.-
Foreshorten Linear Dimenions
I believe the CAD term for this is Clipped dimensions. I think there are programs that support this, but I'm glad S/W does not for the reasons stated above.Jeff Hamilton wrote:
I actually created symbols on the GTOL file for this. (RH , LH, Up and Down arrows). They work in most instances, unless you have to add notes to the dimensional values. The it can be difficut to get the arrows to line up correctly.It works, but I'd much rather have the real thing.
-
Foreshorten Linear Dimenions
Attached is my modified GTOL.sym file. I would recommend saving a copy of your origional file before overwriting it with this. It goes in the Solidworks/lang/English folder. You will have to restart Solidworks to get it to take effect.
Once loaded, you hide your dimension and extension lines and then use the arrows just like any other symbol, such as the diameter symbol, etc. They are at the end of the modifying symbols section.-
Foreshorten Linear Dimenions
***CAUTION***CAUTION***CAUTION***CAUTION***CAUTION***CAUTION***
Once the "gtol.sym" file has been modified and used to create drawings, then the modified "gtol.sym" file will be required on all workstations by everyone who accesses your drawings. This is true for all other SolidWorks users and for those who view your files using the SW Viewer and/or eDrawings, internal & external customers.
This is a widely known problem that most experienced users know about. However, when sharing information such as modyfying the "gtol.sym" file with the community in general, you must consider that there are many newbies & less experienced users.
-
-
-
-
Foreshorten Linear Dimenions
It's up. Let me know if you have any comments you'd like added or updates to the symbols.Jeff Hamilton wrote:
Sure
-
-
-
-
-
-
-
-
-
-
-
-
-
Foreshorten Linear Dimenions
Bradley,
Instead of using a Detail, could you use the Insert > Drawing View > Break function and show both ends?-
Foreshorten Linear Dimenions
I've downloaded the .sym file from fcsuper.com. How do I get this to work??
Thanks
DaveP-
Foreshorten Linear Dimenions
Dave, the instructions are included in the file itself. Please let me know the upload is good (the zip file has the .sym in it)? You can read the .sym with a text file editor. Copy its contents, then open the Gtol.sym file in your lang/english folder. Paste the contents to the end of the Gtol.sym file.David Plowman wrote:
I've downloaded the .sym file from fcsuper.com. How do I get this to work??
Thanks
DaveP
When you start SolidWorks, start a new annotation note, then enter symbol and goto Foreshorten Arrow heading.
-
-
