Show/Erase and created dimensions

[AnkurAggarwal]

Everytime it is imposed on Pro/e users that do not use created dimensions and always use show/erase in drawings. In my company also it is the practice. But every time it seems to be not possible. For example, in cast/machined drawings, sheet metal formed and flat drawings etc. Do anyone has a solution to such problem? I mean how u people tackle with such problem? Thanks Ankur.
This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[PhilipRoy]

Ankur; I'm not sure I understand the problem. Are you saying that every time you use "show dimensions" that it does not work properly for you? From my experience "show dimensions" is an option that references the dimensions from the sketch and or bends that you chose to do in the part model itself. If these two things are done properly in the first place, they will display properly on the drawing. For instance, every time you chose to make a dimension "solid" in the sketch of the part, this will become a reference dimension (ie D23) that can be accessed through the "show dimensions" option. If you carefully choose your dimensions, then only those dimensions will display in the drawing. If this does not answer your question, please re-phrase your question so I can try to give you a better answer. Hope it helps! Phil

[AnkurAggarwal]

Philip, thamks for response. let me raise the question again. We can create dimensions in proe drawing by two methods. One is Show/erase which displays the dimensions of sketch etc. and second is create dimensions in drawing itself (Insert > Dimension > New Ref). The second method is not considered a good practice. Infact, companies strictly instruct their proe users not to use the second method. But in some cases we cannot avoid using second method. for example, in drawing of a machined part (modeled by merging cast part into machined part) and sometimes in sheetmetal flat layouts. How we can use Show/Erase (1st method) everytime and avoid creating dimensions in drawing (2nd method)? Hope u understand my question now. Thanks Ankur

[PhilipRoy]

Ankur; Thank you for re-posting, I do understand your question now. In my experience with ProE, it can be very picky as to what it will and will not display with show/erase dimensions based on how you bend a piece, or how you merge a piece. Basically what I'm saying is that unless you know the program inside and out, which none of us really do, then that would be the only way to get around this problem. In my opinion, sometimes it is inevitable, and you must create dimensions yourself in a drawing in some cases. I have not tried WF5.0 but I hope that it helps to solve some of these picky issues. Sorry I could not be more help. Phil

[AnkurAggarwal]

thanks a lot Philip.

[eric.mills]

Ankur Philip makes good points in his replies. I will say that you can limit the use of created dimensions (ad type) in your drawings based on how you model the part. Many companies use the enforcement of not creating dimensions in the drawings (ad) that way the users will use the model dimensions. It is a best practice style and fully agree with that type of standard. There are times that the dimension just will not show up based on the views and that this is a 3D model; rounds and drafts and good examples of hard to dimension sometimes. On a sheet metal part the flat state could be the first feature of the model and bends added to the model. Then your model show the flat pattern dimension. Best of luck Eric

[CBenner]

It should be noted that in some modules of Pro-E that create enities for you, such as spec driven Pro Piping, there are no dimensions that you can use. "Show" dimensions gives you what is essentially gibberish from a fabrication standpoint. The same is true with EFX (frame builder). In some of these modules, in order to make a print that the shop can actually read, you have no choice but to use created dimensions. Just my 2 cents worth.

[AnkurAggarwal]

u r right eric, but there are cases where I have found difficulty. Let me give u an example. I have casting and machined drawings. In machined drawing, those dimensions will not be shown which are already shown in casting drawing, right. Suppose There is a length dim shown in casting drawing. That length should not be shown in machined drg as it is not to be machined. But I want to show it in machined drg as well as a reference dim. Now if it was "20.00" in cast drg it has to be "20.00 REF" in machined drg. How we can use show/erase in both drawings? Hope u understand my question.

[DavidButz]

Just reemphasizing some remarks made by others: 1. It is excellent general policy to create geometry using the dimensions which should control a part and will eventually appear on the drawing. A very basic example of this is certainly hole location. If a hole is to be controlled, drawn, and machined with refernce to side surfaces, it should be created that way; if it is to be located relative to the center of the part, it should be created that way. 2. However, an absolute policy of this sort does not take into account the real-world complexity of the modelling environment proviced by the CADD tools or the complexity of geometry development itself. There are numerous times when the efficient, sensible method of geometry creation will not use the dimensions which will ultimately be used for drawings and manufacturing control. This occurs all the time. Just one simple example. You are designing a thin-walled molded part where the most efficient, sensible tool to use is Shell, even though you are going to control the geometry by some internal dimension created as a result of the Shell. You will have to Create that dimension in the Drawing. You might be able to "stand on your head" to create the geometry based on the dimension in question, but if it's going to create a much more complicated Model Tree and be much more tedious to create, then the tail wags the dog. Common sense is required.