A new behavior in Creo 4.0 I don't like. Now when using ordinate dimensioning, Creo places automatically the dimensions on the same side as the origin zero. More precisely, this happens when you want to add dimensions to a drawing. I don't understand this new behavior and gives me more job as I have sometimes to place the dimensions not on the same side of the zero. Do you know if there is a way to disable this and come back to the same behavior as in Creo 3 ? Thanks.
Not to disable it, no. It does work better for most cases, as you dimension with pick pick pick instead of pick place pick place pick place, and it aligns the dims. But in this case, not as efficient. If you have a single dimension to put on the other side, you can move the dim after placing (which we understand is more cumbersome). If you have a bunch of such dimensions to make, consider the workflow
Move the base line temporarily to the other side, Ord Dim, pick base line, pick 20 bits of geometry. Then move the base line back.
Ord Dim, pick base line, pick 20 bits of geometry that you want to dimension on the other side, then look in the Drawing Tree and select the last 20 dims, and move them in one move operation.
I will ask after the possibility of ending ord dim creation with the recently-created dimensions selected, which would allow the second workflow to skip the step of finding the dims and selecting them. I'll also ask after the possibility of allowing a pick in open space when you've just made an ord dim and are possibly about to make another one, with the meaning of move the just-created dim to that point. However, I cannot promise anything.
With Creo 3.0, it was not pick place pick place... it was pick pick pick then place all the dims created. So we could do one side of the part then the other side.The click gain with Creo 4 is null because we have to move the base line before creating ordinate dims on the other side of the part where before we just had to choose the side after creation.
I had discovered in the time between my question and you answer that the dims are always placed on the same side as the base line so I started playing moving the base line.
Creo 3 behavior was not really time consuming, now it is.
I'm really open minded to change, but in this case I don't really get it.
When we create ordinate dimensions, we haveto pick first the base line or an existing dimension. The improvement could be to place the new dimensions aligned on the same side as the first dimension or base line we picked. What do you think about this Matthew ?
Sorry, getting the various people to take a look took a few days. I've now got their answers and can update this thread.
First, kudos for cleverness for realizing there was a bit of information (the dim selection before picking geometry to dimension) that could be leveraged!
Second, I'm happy to report that the applicable PM and Dev people confirmed that it would be feasible and desirable. We're preparing the suggested improvement, and expect to have it in M020.
Thanks for the suggestion!
Hello, i'm an Italian drawer. I have the same problem, with complex drawings it's impossible to work. Do you have any solutions? I try also release m40 but the problem is the same. Thanks to all.
Hello, why this post is dead and anyone reply?
I work on complex drawings and i'm in serious difficulty.
With Creo 18.104.22.168 the problem is the same. I want an option on config that disable automatic allignment.
This problem is driving me crazy! For complex drawings, it is extremely slow comparing to previous versions. May be in simple drawings, when everything is lined up, nice and clean (e.g. drawings from PTC tutorials) it could work fine. However, in practice, holes are not aligned, drawings are complex and the only way to place all ordinate dimensions is to divide dimensions into clusters and place them to all sides. I am tooling designer, I do complex designs of progressive die tools with quite big plates, drawings has to be finished with ordinate dimensions. In 20 years, I have finished thousands of such drawings. And believe me, new version of CREO (our corporation is on CREO 4.0 060 now) is far worse than previous, it ruined my productivity in ordinate dimensioning. Even in Autocad it is easier to do ordinate dimensions now. If someone from PTC reads this, please, look at attached drawing and tell me how the hell I can finish such a drawing in newer version of CREO!!!
I can send you a model (to attached drawing) and try for your self how long it will take to replicate same drawing in CREO 2 and then in CREO 4...
My name is Michael Fridman and i am the product manager for detailing at PTC.
Could you please elaborate more on the points that takes you longer to create ordinate dimension
which part of the process makes it longer than before?
here is comparison of my steps now and before.
In CREO 2.0: 1.select origin, 2. select all entities in one area/cluster, 3. place and align all dimensions IN THAT AREA or rearrange them after this step, because all dimensions are still selected. Repeat these steps again and again in as many areas as I need, because I dont want to have all dimensions on one row.
In CREO 4.0: 1. select origin, 2. select all entities -right in this step all dimensions are instantly aligned to origin dimension (which I dont want), 3. finish dimension with middle click (not able to decide where), 4. manually rearange dimensions to required areas - another problem here is, that after selecting and placing dimensions they are NOT SELECTED, so if they are mixed with previously placed dimensions, I have to select them one by one again to rearange...
Please, take a look at my drawing, it is quite easy to imagine how difficult is to rearrange all automaticaly aligned dimensions. I can send you model of that plate, try to replicate my drawing and it will be clear what I mean...
" another problem here is, that after selecting and placing dimensions they are NOT SELECTED, so if they are mixed with previously placed dimensions, I have to select them one by one again to rearange..."
For this part of the problem check the config option -> select_newly_created_dims to yes (CS272125)
...Auto Ordinate Dimension in CREO looks great just on simple drawing as showed in the video. Try Auto dimensioning on large plate with hundreds of holes in random position (not in line) and result is disaster. See TIF picture from my post 07-02-2019 02:14 AM. It is one of my typical drawing from on one of my progressive die tools. It is not working on complex drawing like that example. Time spent on rearranging auto placed dimension is in par with time spent on one by one dimension method... In CREO 2.0 I was arround 40% faster (I did time comparison) with ordinate dimensioning.
Yes, it was simple example.
For your complex view you can try manual steps. As you can see on the video, first create base line, move this base line to correct potion and then create new dimension (with CTRL you can select more references). Then move base line to new position and repeat these steps.
I know this method and I do it exactly like that. Anyway, it was better in CREO 2, where I was not forcet to move base line here and there. I used to place one cluster (row) of dimensions anywhere...
They included the old "Creo 2" functionality in Creo 7.0. It should also be included in Creo 4.0 M120 with new DTL option:
Yes this is correct. This functionality will be available with Creo 22.214.171.124/Creo 126.96.36.199/Creo 4.0 M120
It will be available only for the case that the detail option: "ord_dim_standard" is set to "STD_ANSI" because ISO do not support misalignment of the ordinate dimensions with the baseline
In addition, I just wanted to point out that we (PTC) are indeed paying attention to the requests that are provided in this platform (community site) and we are providing the necessary enhancements and fixes when we can do so.
This fix is a great example because it was picked up from this thread exactly, so your voice is definitely being heard 🙂
Is PTC angry with its customers?Punishing us the way they want, by changing an already established work flow.
Making drawing is soooooo difficult in CREO now.
Everything Everywhere has just to many clicks...just change the software to Solidworks or something else.
I agree, sometimes you want this behavior but for my most work (99%) creo3 was better. Might I suggest to PTC that when they arbitrarily change behaviors, enable a configuration option to enable previous workflows. This will allow us old timers to evaluate OUR best workflows