[kawman]

I hope you guys aren't getting sick of me and my problems! but anyway, i have a model here that has a hole in it, it was drawn in inventor, and i just had our engineer open it and it looks fine in inventor, not the case in bobcad, so how would i go about fixing this? i havent done alot of 3d modeling before, and when i did try it was with solidworks, so im a kinda lost on how to approach this.

[kawman]

ok, i opened it with 123d, and resaved it, then it looked fine in bobcam, but im wondering what is the issue? why do i have to open it with another program? what file types work best with bobcam?

[SBC Cycle]

This morning I had a (rare) problem with a SolidWorks file. I opened it in BobCAD and there were numerous surfaces missing. I immediately saved it as a STEP file and then opened the STEP and it was fine.

This is a question for the Burrman. I know he has explained it to me before but I can't get my head around it.

As you will recall, I despise Inventor files and so did the engineers who used it. It's easy to screw up the constraints I'm told and make the drawing "blow up" into nonsense.

[kawman]

yeh the burrman is the one who told me about 123d, and im also really starting to hate inventor files, what 3d file types do you work with most? im just wondering if maybe iges, xt or something else might cause less problems

[warrenb]

You basically just do what you've already done. Find a format that works and stick with it.

IGES is the oldest and buggiest of the formats. I have had lots of problems with parasolids in BobCAD.

I have had no problems using STEP with BobCAD v24. Just make sure your inventor engineers export the same.

[SBC Cycle]

why do i have to open it with another program? what file types work best with bobcam?

I prefer STEP, even with if I can get a SLDPRT (SolidWorks) file. My armchair guess as to why it works better than others is that it has a fairly clear and rigid structure and set of standards.

Not that every CAD/CAM maker honors the standard, but it's closer than most.

[SBC Cycle]

You basically just do what you've already done. Find a format that works and stick with it.

IGES is the oldest and buggiest of the formats. I have had lots of problems with parasolids in BobCAD.

I have had no problems using STEP with BobCAD v24. Just make sure your inventor engineers export the same.

+1

Didn't see this post but I agree 100 percent

[BurrMan]

Hi sbc,
It will depend more on the app the model is comming from. For Autodesk, I would use the SAT (ACIS) format for best results. Solidworks would be STEP for sure (For "SOLIDS")

The IGES format will be more "surface" oriented and usually transfers as sperate surfaces, then the importing app will "stitch" solids where it can (and some have options to leave them as they are. The "stitching" in one app comming from another is where you get e "bugs" you speak of, but it is most likely related the something else. I often use IGES to "fix" this type of stuff.

For Kawman:
Regarding your previous model and your engineer with inventor. As the last thread pointed to, the bad trims were not apparent or present in the autodesk apps (Inventor-123d etc) But were in many others. I would suggest this. Speak with the engineer and look at a couple things together.

1. Is he working in some other units than what you are expecting or opening the files in? (There may be some scaling happening during transfer that is throwing off the tolerances defined)

2. Does he have some specific tolerance set in Iventor that may not be enough to produce the proper trims for the parts he is making? (I noticed in the last BobCad file that you have tolerances set at .001. Although this "seems" like it is tight enough for your machining purposes, the model had several small, slivery surfaces created from either poor modeling choices, or autodesks ability to fillet into areas that create this. These little surfaces can have the trim regions start to fall outside of .001 and cause these types of join problems with the surface trim boundries.

Thats all I have. But mostly, ask him to send you a SAT file from the native Inventor model and see if this goes away for you. OR, if the originating model is not "native" from inventor and your engineer, but a result of him bringing the model in from someone/somewhere else, then you inverstigation can go to that previous point in time, with the same methods as described above.

[warrenb]

I prefer STEP, even with if I can get a SLDPRT (SolidWorks) file. My armchair guess as to why it works better than others is that it has a fairly clear and rigid structure and set of standards.

Not that every CAD/CAM maker honors the standard, but it's closer than most.

I have never had luck opening a solidpart part in Bobcad. I know it says it will open it but I've never had it work.

But regardless the post is on what to do with Inventor files. Inventor handles SAT and STEP.

[BurrMan]

So I downloaded and looked at the SAT model you supplied in this thread.. It appears to be a SAT file from "TransMagic"?

Could you review if you have supplied a file exported from Inventor?

Maybe you need to look at the full history of the models you are getting.

Are they actually created in Inventor, from a single person? Or are they being passed between different systems? Is someone performing secondary tasks on the model with transmajic like "autorepair" or something?

I could show you areas on the model that are the "little slivery pieces" from poor modeling that may be causing your problems if you want to see those.

[neilw20]

The Boolean operation on solids failed.


Modeling Operation Error:
Inconsistent face boxes - probably faulty edge boxing.
SLICE failed for selected solid.

Welcome to the wonderful world of fillets, not intersecting properly.
Just one click creating something visually can select a wrong point creating corrupted geometry.

Yes, Transmagic?

And various packages offered to repair it.
Importing into some (read that as try many) package, repairing and exporting as a Parasolid seems to work reasonably.

[kawman]

Yes burrman that file was ran through transmagic to try and repair, the holes, which like you said are usually on fillets, Also yes i would like to see the spots that point out to bad modeling, but there lies the problem, im sure my machinist counterparts will agree, i cant just go in there and say " this guy on the internet says you suck" the engineers, ours and outside ones dont seem to see any issue with their models, as for the models themselves, we build machines for the auto industry we are not a tier 1 supplier, so lord only knows how many people have worked on these models, usually i see, we get a part file then we need to make a nest to hold that part, so im not exactly sure how they come up with the nest's, so if this comes down to "better modeling" that basically means i have to deal with it :drowning:,

[neilw20]

You need to deal with the creators and get them supply proper models in a form you can use them.
I can open that ACIS file, and it has hollows, windows and discontinuities.
Getting something to 'repair' which seems to have happened to this file often destroys data.
I see and deal with this all the time. Cross platform file transfer is painful.
I don't use Bob-cad so really don't know what it will accept.
Find out the original source program and ask Bob-cad the best way to use a file from that program.

When ACIS file is saved with inventor/ACAD, it is important for the user to select and orient what is intended, exactly.
Don't include multiple parts in the same file.
And it is nice if UCS is selected that gives a sensible 0,0,0 and orientation for the intended user.
XY with Z upwards is suitable for VMC. That saves some work importing, and use the lowest ACIS version possible. The more complex it gets, the more screwed up it often gets.
I note, that in that file, 0,0,0 is off in the weeds somewhere, and Z is stupid, at least for VMC.

[kawman]

Thanks for the input Neil, i agree about part orientation, some times its 1000 inches from 0,0,0,. You guys are always a big help

[BurrMan]

Yes burrman that file was ran through transmagic to try and repair, the holes, which like you said are usually on fillets, Also yes i would like to see the spots that point out to bad modeling, but there lies the problem, im sure my machinist counterparts will agree, i cant just go in there and say " this guy on the internet says you suck" the engineers, ours and outside ones dont seem to see any issue with their models,

so if this comes down to "better modeling" that basically means i have to deal with it :drowning:,

Looking at the transmagic model may be misleading, but it had some of the same issues as the first one you posted... It's not "filleting" that is the issue, although filleting would exacerbate the issues.

Here is a look at the negative x side of the model:



I drew 2 green lines where it appears they have joined 3 seperate bodies into one. Nothing wrong with this, but a slight mis-alignment will cause issues. I the 1 area, you can see the slight mis-alignment. This is caused either by 2 bodies being joined that had the same non-contiguous surfaces, or by poor alignment of the 2 bodies. The filleting exagerates the little malformed edges that are results.



In area 2, I drew a green arrow pointing to an area that depicts the bad trims... You see the poor alignment in the area, then note the trim edges down there from the fillet. There is a small area between the 4 surfaces that have "NO TRIM BOUNDRIES".. These will create the problems you are seeing.



That little gap is .0019.This can fall under the tolerances of commands in the program, like "FILLET".. That little gap wasnt created by fillet, but by the mis-alligned previous operation.

I wouldnt suggest that the modeler "Sucks" (Maybe a bad move from the machinist anyway, from a good relationship standpoint). He may not know anything is wrong. Like we see, autodesk shows a "great model". He needs to be shown that there is an issue so he can address it.

I dont think it's a translation issue either. I think the modeler can find something in his workflow that originally created the tiny mis-alignments that would solve many of the issues.

i agree about part orientation, some times its 1000 inches from 0,0,0,.

This is an indication that the part is being designed in a unit system other than yours. Like "Meters"

This could help to explain the issues you see with joining failures. The tolerances defined in the translation seem to me to not be in step with the model presented. This would be a unit system mismatch and you would see nothing but problems with it in any other app. With this, I had suggested that you sit with the modeler and discuss the defined units and such.

Of course, all this depends on the modeler being willing to address things with you. But a modeler who is not willing to discuss that there may be an issue you need addressed, "SUCKS"!!! It's not "BobCads" fault...

[neilw20]

Nice work BurrMan, but your attachment links are a little dead ended.
Thanks, That's fixed.
I saw irregularities, and too many, and my standard response is reply to the creator.
Even an end with a huge hole. Is it just surfaces?

[BurrMan]

Nice work BurrMan, but your attachment links are a little dead ended.

Refresh your page. I fixed them.

[BurrMan]

I saw irregularities, and too many, and my standard response is reply to the creator.
Even an end with a huge hole. Is it just surfaces?

With the last model Neil, the issues you see may be more misleading, because someone ran it through transmagic. Transmagic is a powerfult tool, but you need to know alot about it, or you can just make things much worse.

If you refer to the first model that Kawman posted as a much more "What he's dealing with" model... It will come in as a solid object, however, further operations fail, in many other apps too. Also, you can just zoom and look at it and see what "I recognize" as a tolerance issue (The underlying root of the problems with his inventor models). It looks more like a mismatch, where the underlying geometry had been scaled/not scaled at the same time the tolerances have been not scaled/scaled. usually, it starts where one system is working in a particular unit and it's transfered/translated to another system unit without care or understanding.

[EDIT] The "previous model" I keep refering too is here:

http://www.cnczone.com/forums/bobcad...ter_marks.html

[EDIT]

[neilw20]

I always overlap surfaces before I combine to ensure there are no gaps.
Need to trim something with complex faces.
I slice until the simple part remains, do the operation and rejoin them.
Never have problems. But I've seen too much doing it drag and drop etc, and WYSIWYG just doesn't hack it. It hacks it.