When I am creating drawing packages for engineering change notices I put all drawings in one draft file until I release package upon approval of ECN. Most drawings are in metric format, but a few legacy drawings are in inch format and management does not want to change these to inch format. The inch format draft tabs are set to the dimension style of inch format when needed. What I have encountered is that when I have a dimension that has tolerances that do not agree with general tolerances on drawing and need to be keyed in. Using Unit Tolerance in pull down, with dimension style set to inches is that the keyed in tolerances are still being applied as metric, if I key in say 0.04 the dimension tolerance is displayed as 0.002 (see attached jpg file). The units in the draft file are in metric format. All settings in the style for the dimension are set to what I beleive is correct.
Is there a setting I am missing that would have the keyed in tolerance display as keyed in rather than being converted to metric?
When draft file units are changed to inches, tolerances for inch dimensions display as keyed in.
Copy of my draft template attached.
Gary Dinges | Mechanical Design Engineer II | Probes & New Product Development Emerson Climate Technologies | Therm-O-Disc, Inc.| 1320 South Main Street | Mansfield | OH | 44907 | USA T +1 419 525 8554 email@example.com
You kind of lost me here "...I put all drawings in one draft file..." but when I open your draft and change the file units the on-screen dims don't change but the tol values in the ribbon do.
I have multiple tabs (sheets) in one draft file. Most files are metric format, a few are inch format. The same draft file at times has some metric and some inch format sheets.
I made an example file to illustrate what I am doing.
Two screen captures attached. One is Metric example and other is Inch example. Both are in the same draft file as shown by tabs in lower left. There is a different background sheet for metric & inch files.
The dimension and tolerance values in the metric tab function as expected. Tolerance is keyed in at .10 and displayed in dimension as 0.1
The dimension value in the inch tab functions as expected, dimension style set to Ansi inch. The tolerance does not. It is keyed in at .10 and displayed in dimension as 0.00039 (display decimal value was adjusted to 5 places). Screen capture of the Ansi Inch.
My reason for using one draft file for multiple sheets is that I find it easier to switch between needed sheets as I create drawing package. Some files I have contain uo to 10 tabs,each with a different draft file. Some parts, some assemblies, some metric, some inch.
The units value for the draft file is set to Metric in examples attached, if I change units to inches, the tolerance function as expected for Inches and incorrectly for Metric.
ST7 with MP10
I think I understand.
With the file set at mm units:
for inch dims it divides everything by 25.4
but the tols still display:
in original mm in the ribbon
in converted inch in the dims
With the file set at inch units:
for mm dims it multiplies everything by 25.4
but the tols still display:
in original inch in the ribbon
in converted mm in the dims
OK. Think I understand what you have going on here. He is the fundamental thing:
1. There are FILE UNITS -- these are independent of any dimensioning style etc. Anything you key in in ANY field (including tolerance) will use these units if you don't add any qualifier to it.
2. There are DIM UNITS -- these are the units of the dimension value.
So what is happening is the tolerance fields are taking input in the FILE UNITS and it is being converted to the DIM UNITS.
Because there is only one set of FILE units, you cannot key in .01 and expect it to be Inches in one dimension and mm in another. So mixing the two types in a file can cause confusion.
There are two cures:
1. When you key in the tolerance field, and the file units and dim units do not match, you will have to key in the units. Example: file units is INCH. Dim is in MM. When you key in the tolerance key in ".01 mm" (you have to include the mm to let it know you mean mm, not inches).
2. You could use "text based" tolerance. This was the only option in Solid Edge for about 10 years. It just takes whatever you key in and uses it literally. The problem with this option is if you want to convert mm to in or vice versa in the future, you cannot -- cuz its dumb text.
PS> Been doing Solid Edge for 20 years, and I think the is the first time this has come up.
I understand your explination, but considering tolerance units are set to match the primary dimension values (inches or metric), it seems reasonable to expect a keyed in value to behave the same as a system generated value.
In case anyone is wondering why I have all these files lumped in one draft file, I am working on a large program to move some of our product lines from China to Mexico. The Chinese group has never been forced to comply with many of our standards for various resons. The drawings are of less than stellar quality, appear to be done in an unknown CAD system, then imported into AutoCAD. They generally outsource sub-assemblies to another vendor, so many componenents don't have full documentation such as clear wire specs, terminals housings etc. I find it easier to have the drafts in one common file, so as I work through creating models and assemblies I can more easily swap back & forth between individual drawings, rather than having a seperate file for each. Once I have ECN approved, I then split the common draft file into seperate files for archiving & distribution. May not be the way it is normally done, but it works for me.
Now that I am aware of this issue, I will work around it. I haven't tried it yet, but as I am typing this I am concerened what will happen to keyed in values when I split files. As long as I don't change units on the oddball inch in a metric based file I am OK, but I have to look at ramifications of future revisions being done by another person not aware of this 'issue'. I will need to go back and check the few inch based files I have done to verify they are functioning as intended.