Pro E Question

[mman10]

When importing a model from Pro e that has unilateral tolerences for example plus/plus or minus/minus. Is there a method to import the geometry to take this into account. The geometry always is at nominal where the tolerence will be +005/+010.

[chip]

quote:

---

+005/+010

---

Do you mean +.010/-.000?

 

If the model is drawn in the median of the tolarance. That is what should be translated into, lets say MasterCam in this case.

 

If you have a Bore 1.000 +.010/-.000 the designer drew the model at 1.005 that is what should be translated.

[Neal Z]

Welcome to the forum from a fellow Pa user. Here at my work, I import ProE all the time. Not sure what your asking. Wouldn't the geometry come in to size, like what it was drawn to in ProE? I'm sure someone here can help you out. If not, Whose your dealer? Prism Engineering or Innovative Solutions. One of them should be able to help you.

[mman10]

The model is drawn at Nominal but the tolerances can be +.005/+.010 or -.005/-.010. These are specs that are used in Europe and the parts are manufactured both here in the states and Europe. For example 1.000 +.005/+.010 thus the hole woul be 1.005/1.010. I've been using Mastercam since version 6 pretty sure nothing it can do but does anyone know if pro E can? Engineer states certain features can be toleranced this way but not drawn in the model.

[HevyMetl]

Converting between the two on a daily basis has caused to ask this question as well. The answer I was given was that a translator ignore all user defined values. ie tolerances, notes, ect...

 

If I want to use the median of the tolerance to be able to make good parts I have to remodle a copy that way, as to not affect the engineers modle. I know it s*^&$s.

[Paul McGarr]

I can't answer for ProE, but I don't believe that Mastercam will ever look at part tolerancing and alter a model because of it.

 

Is it a European thing to dimension like that? I've never seen it. I would think that the hole you used in your example should have been modeled to a dimension at least within the tolerance. An example of that would be a 1.005 hole +.005/-.000, or 1.0075 +.00025/-.00025, etc.

 

Tolerance by definition would suggest an acceptable amount of deviation from a given value. That's not the case in this example as the given value (1.000) is not even acceptable.

 

That seems real odd to me. Has anyone else seen dimensioning like this? At this point, I am just curious if that is proper practice, even for Europe.

 

Paul

[IntegrexMan]

We deal with lots of European drawings and models here. They are all Unilateral toleranced and the models are drawn to either the upper spec or the lower spec not the mean. A major pain the a**. There is a software package we are investigating that will alter the Pro/E model to make it to the mean so when we bring it into MC, the are correct. I will get the name of it for you.

[mman10]

IntegrexMan, I work for the same company. I am in the Tech center prototype shop. If you can get me the name of it that would be great.

[kwolf]

quote:

---

There is a software package we are investigating that will alter the Pro/E model to make it to the mean ...

---

Very interesting, sometimes changing a value by very very tiny amount can cause a feature to fail in a solid modeler. I wonder how this program will interpret such tolerances, prolly it should rebuild all the features again, this means it should work as a PTC plugin.

 

I saw a demo by TopSolid years ago and the guy told us the CAM side can machine the geometry created by CAD side with median tolerance.

[Bruce Caulley]

We have our designers draw to mid tolerance. Most engineers or designers don't understand the problems that nominal dimensions cause.

 

Bruce

[Müřlıń®]

Ahh the old slot dim blues......Dont ya just hate converting 100 slots to hard ones heh....

 

OH BTW, I have never heard of such a thing as looking at the tolerances.

 

I use PROE/MC and what you draw is what you get. Depending on the system tolerances of course.

[kinglouie V]

I have seen an italian drawing dimensioned

like this before. seems to be very euro.

+/+ -/-

[pronc]

Integrexman,

 

Quote:

-------------------------------------------------

There is a software package we are investigating that will alter the Pro/E model to make it to the mean so when we bring it into MC, the are correct. I will get the name of it for you.

-------------------------------------------------

 

 

you can set all the dimensions to nominal before export the model out. go to "setup", Dim bound", "set all", "nominal", "done". Hope this helps.

[HevyMetl]

pronc,

 

Are you sure that it changes the actual size of the part? The problem as I understand it is that mman10's part is designed at the bottom side of a onesided tolerance.

[mman10]

Actually the problem is the part is modeled either above or below the tolerance. For example

1.000 hole +.005/+.010 meaning the hole is not 1.000 but 1.005/1.010. I tried the method pronc suggested but it did not work.

[pronc]

Mman10,

 

sorry. i made a mistake. you should set it to "Middle" not "nominal". i tested it. it worked.

[pronc]

Hevymelt,

 

yes it works. That will changes the actual size of part. i already proved it out as i stated above. what i did was open up a part, make sure the tol was set up correctly. set the dim bounds and regen the model. that was it. i use this alot in manufacturing for r&d study but not for exporting to mastercam.

[chip]

Let's say you have a bore 1.00 at the bottom of a pocket. Bore is near the wall and a has fillet at the top of the bore.... If you set a tolarance and the computer adjusts the profile of the bore and now it can't create that fillet? there are a lot of circumstances that adjust the entire part... I would be curious to see how that works. I'm not saying it doesn't. Pro Engineer is a power house as far as modeling... I'm just saying, I would be curious to see it.

 

quote:

---

When importing a model from Pro e that has unilateral tolerences for example plus/plus or minus/minus.

Is there a method to import the geometry to take this into account

. The geometry always is at nominal where the tolerence will be +005/+010.

---

Sorry MMan10. not that I know of...

[pronc]

in the particular case as Chip described above it still works. But of course there will be cases when proe fails to regenerate.

[mman10]

pronc,

 

Your method worked for us as long as we did set selected not set all. Thanks for the help as this is an unusual problem.

[kwolf]

Sorry to hijack the topic.

As an amateur software programmer in old days I'm really interested in how some CAD/CAM systems can do this. Please let's know if you have something in your mind.

 

I think the best way is to use an integrated CAD/CAM. The CAD-side can generate tolerances for each face and trasfer it to CAM side, the user can then use those numbers in "stock to leave" parameter. So there's no need to rebuild or recreate geometries. Maybe for XI.

This method can be used for simple geometries especially for analytic geo now.

[Müřlıń®]

Yo...Pro...hey thats pretty kool about the tolerances....learn sumpthin' every day in here.

 

Question...I was looking at the tolerance setup and couldnt see where to set up just a single dim tolerance. Could you point me in the right direction

 

From what I could tell it was kind of a global setting..

[pronc]

Murlin,

 

instead of "set all" try "set selected" then select the feature. some dims will show up. select the dimension you want to set. hope this helps.

[Müřlıń®]

Ahhh...Gocha...Proe is an awesum little tool...

 

The advantages of Parametrics.......

 

Thanks....

[Verisurf - Ernie Husted]

We sell Inspection software to all types of industries, I can say that we have to allow a User to inspect a part that has off sided tolerances, Some of the cases for one sided tolerances are because of some kind of process allowance, such as plating. In some cases we inspect parts that have +.05/+.075 prior to heat treat, etc.

 

I wish that we could translate the tolerance information from Pro-E into Mastercam, I believe this simple feature would change the Manufacturing World as we know it now., it will save tons of time by eliminating the need for a blueprint.

 

Does anyone know how to get the tolerance information out of Pro-E?

Maybe a file that has each Feature name with Tolerance info.

 

Happy Thanksgiving

 

Thanks

Ernie Husted

Verisurf Software, Inc.