Pro-E is driving me crazy

[MukaSingh]

I've been using SDRC then NX for a long time and now my company wants to switch to Pro-E. I've been working on some of the tutorials. Can someone tell me how I can delete dimensions? I draw my sketch and I select the one by one icon and it automatically add the dimensions to the sketch. I want to re-dimension the sketch using my own dimension scheme. How do I delete the dimensions and add my own? I also tried the Normal dimension with no success.

Thanks for any help.

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[SteveChoryan]

are you driving the dimensions in the drawing from the model? meaning are you hitting the show dimensions button and showing them?

This is the prefered method as you know they are real dimensions and not faked. In my opinion i would change your model to agree with how you want the dimensions to show up in the drawing.

Also as an fyi

If you hit Show dimensions on a view it will show all the dimensions, you can then select the ones you want to keep on that view.

then go to the next view and hit show dimensions and it will bring in the ones you dont have displayed on the first view

also

to get rid of a dimension that you have shown, right click it and go to erase and it will disappear.

then you should be able to use the normal dimension tool to put whatever you want on there.

if you need more help let me know

i can make a quick video tutorial for you

here is the quick video i made

http://communities.ptc.com/videos/1338

if you need more help feel free to ask

[GregFrankland]

If you are in Sketch mode, you can just start dimensioning the sketch as you would like to see it. As you add the new dimensions the automatic dimensions will disappear. The sketches in Pro/E have to be constrained at all times, and adding the new dimensions should make the automatic ones disappear. Also note that there are three types of dimensions in sketcher:

Weak dimensions - The automatic dimensions will start out this way, they appear gray in the sketch window.

Strong dimensions - The dimensions you create will automatically be strong dimensions and they show up as yellow by default. If you like a weak dimension and want to make it strong you can make them strong through the RMB pop-up menu

Locked dimensions - If you have a dimension in your sketch that you want to lock and not let it change when dynamically dragging your sketch, you can lock the dimension using the RMB pop-up menu. These dimensions will appear orange by default.

-Hope this helps,

-Greg

[MukaSingh]

Thanks for replying but I've been trying to add a dimension for 3 days now on a simple sketch and can't do it yet. I used SDRC for over 15 years, NX for over 3 years and also had a stint with SolidWorks so I do know something about dimensioning. When I try to dimension the sketch I see a cyan color painting the line in my sketch. I have to wait for this to finish before Pro-E respond to my mouse/command. This is very frustrating. I used to draw sketches and dimension in seconds but with this software I have to wait for the painting to finish. Sorry for my ranting but we are in the process of evaluating Solidworks and Pro-E and I wanted to get a jump on things before we get formal training.

[ScottArchibald]

This sounds like another problem that is not ProE. I had problems with

models painting when I upgraded a system. The graphics card needed

a software upgrade (free download) to work.

[ShawnPete]

Your problem sounds like one I have had in the past. If you are using the windows plug and play monitor driver, try installing the manufacturer's driver for the monitor you have. Make sure your graphics card driver is uptodate. If you experience forced closings of Pro/E, it might be from a graphics card that is undersized for the job. When we added a second monitor to our designer's workstations, Pro/E started crashing consistently. We had been using 128mb graphics cards and realized that we were overworking it with the second display. Upgraded our all our cards and - voila - no more crashes !

As far as your original issue, are you in part or drawing mode? If you are sketching in part mode, the weak, automatic dimensions disappear as you add your dimension scheme. However, once you add a dimension, you will get an error if you add a competing dimension. You can choose to erase, reference one of the competing dimensions, or remove constraints to address the error. If you have a dimension you would like to replace with similar dimension, you can avoid the error, by using Replace(?) dimension from the Edit menu.

If you are in Drawing mode, and you have shown dimensions automatically, you should go back to the model to change your scheme. The use of created (driven) dimensions, should be kept to a minimum. I tend to use them only for reference, or dimensions impossible to create directly in the model, such as an overall dimension of an assembly. However, if you must create dimensions, you will need to erase the original shown dimensions, as just adding created dimensions will not remove the model based ones. Do this by selecting a dimension (or multiple dimensions) and choosing erase from the RMB menu. (Shown dimensions can only be erased as they drive the model, created dimensions can be deleted or erased.)

[SteveChoryan]

ive went ahead and made you a basic modeling tutorial. I hope this helps, should explain a lot of your dimensioning questions

http://communities.ptc.com/videos/1353

[BillDaugherty]

Amen to that !! Check with PTC and see about the hardware/driver combination you are using. That is what they do. They should be able to help.

[VitaliyTimoshen]

...NX for a long time and now my company wants to switch to Pro-E

...accept my condolences... According to my observations, PTC today looking only to people with money. Ordinary users they are interested in the least. Be prepared for bad surprises & time wasted.

[brthompson]

Hi Muka,

I think your problem might be that you're trying to delete the dimensions that Pro/ENGINEER creates automatically for you, when actually there's no need to delete these dimensions at all. The automatically created dimensions in any sketch are called "weak" dimensions, which will be used to define/constrain the sketch if you are fine with how they were created. If you are not - and I can see that you're not - you simply need to create your own dimensions and the automatically created "weak" dimensions will be replaced with the "strong" dimensions that you created. Any "strong" dimensions can be deleted, but then another weak dimension will automatically be created to keep the section constrained.

I hope this helps!

Brian