I opened an ipt file (originally a stp file) in Fusion for editing, made some changes, brought it back into Inventor and it has grown by a factor of ten. The default metric units in Fusion for some weird reason appear to be centimeters instead of millimeters. Could this be the problem? Is there a way to set the default units in Fushion? As of right now, I can't use Fushion to edit anything that was originally created in metric units.
Engineering manager, T-mar Industries Ltd
Inventor Pro 2012, win 7 pro 64bit, dell t3500, xeon W3580, 12 gigs, radeon 5870
Many thanks for reporting the issue. Here, I want to confirm your step “brought it back into Inventor”, did you import Fusion files into Inventor, not use change manager addin? If yes, it does have the issue. And Inventor side has known that. They would improve that in future.
Fusion can set the default unit from right corner Unit list. For Inventor and Fusion integration, there is another workflow named Change Manager. I think it can solve your issues. The workflow as below: Create a part in Inventor (unit as mm)àOpen it in Fusion and edit it (set unit as mm),and saved as DWGàOpen the DWG in Inventor. Here, you won’t see the issue. And model keeps the same size.
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I don't have autodesk inventor (and I am an architect so I have little need for it), but I recently was given a job to make adjustments for some 3D objects from a client. Unfortunately, I am not given any information as to what program was used to make the objects, just the STEP files containing the objects.
I downloaded the Inventer Fusion trial version with hopes that I can make minimal adjustments to these objects according to my client's needs.
My problems thus far:
Fusion doesn't seem to recognize the imported shapes as faces and I can't seem to manipulate them easily. Whenever I want to bore a new hole I select the hole option and hover over the surface I want to bore and it won't recognize the surface to bore.
I can't seem to move or adjust any of the existing components (such as previously bored holes).
Is there a way that I can easily convert the imported STEP files to accomodate the Fusion software for these adjustments or is Fusion not meant to adjust existing documents such as these?
If not, is there anything you can recommend for me to be able to complete these tasks at hand?
Thanks for your help!
Can you attach the original STEP file here?
Something doesn't sound right.
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Still waiting for -Draft option on any Rib feature.
I tried to send the original file, but apparently this forum doesn't allow .step extensions. Then I zipped it and found out that the file is too large for sharing here.
Is there any other way I can get the file to you?
Based on your comments, your problem may be due to the model not being a solid body. Every solid body has a corresponding entry in the browser. If the model contains any surfaces (which includes single surfaces and surfaces that are stitched together to form quilts) there will be a browser item called "Surfaces".
The fact that you couldn't pick a particular face to create a hole suggests that the face belonged to a surface body. In such cases typically you need to convert the surface bodies into a solid body. There is a command called Validate which would create a solid body if the input bodies can be formed into a watertight set. However, model repair is generally not a trivial task.
Could you please show a picture of the browser (showing the solid and surface bodies) when you open this model in Fusion?
What you are saying sounds about right. I tried to mess around with the stitching and the quilts, but I couldn't manage to get any successful changes (keep in mind I am very new to fusion and have only previous experience with Autodesk's architectural softwares).
Here is a snapshot of the Browser as it appears when I open the file in Fusion.
What do you think? Is there anyway I can convert these into solid-bodies?
I don't want to to discourage you, but what you are attempting is something that may be beyond what someone who is new to solid modeling could handle. But let me offer some hints:
1. You model has 69 bodies, consisting of 24 quilts and 45 unstitched surface bodies. Your objective is to stitch as many of them together as possible. If you stitch 2 quilts which are touching each other you would get a single quilt. Try to progressively build a single quilt that envelopes a solid body.
2. Use the validate command to stitch quilts and unstitched surfaces into larger quilts. I sometimes set the Checking Level to be "Basic" and the tolerance as high as 0.2 mm to help successful stitching.The Stitch command also can be used to stitch surfaces and quilts together. It is particularly helpful in showing which open edges would be stitched together, and which ones would remain open.
3. Use the "light bulb" to control visibility of each quilt. Turn off visibility of all and turn visibility on one at a time, so that you can selectively stitch the bodies.
4. Use the "Reverse Normal" so that the all surfaces have the grey side on the "outside".
5. Use the "Patch/Merge" command to create surface patches to fill "holes".
So, as I said this can be hard task. But I suggest that you give it a try. Sometimes I have been lucky to fix a model in one go, by picking all the bodies and applying the Validate command on them. Good luck!
Thanks for your help!
I have been working on this file and I have been somewhat successful converting it into a solid. I have still been struggling with some of the other parts of the model however.
1) I quilted the upper portion (quilt 62:148) and validated the quilt which said was successful and no problems were found in the validation process. But still the quilt remains and it wasn't transferred into a solid body. Why is that? Should it become a solid body with a successful validation?
2) After I successfully created a solid, there were two things, the first I was left with the lower surface of the model as an "intersecting surface" and no matter what I tried, couldn't stitch or validate that surface to the successfully created 'solid body'. The intersecting surface doesn't touch anything but what was created in that solid body.
Also, I am unsuccessful in any attempt to make adjustments to the solid body after it's validation. It will let me select the faces and perform actions like push/pull and bore 'hole' but the changes don't follow with the actions. Is there something I could be overlooking?
Thanks for all of your help so far! I greatly appreciate it!
A quilt can pass validation (no errors reported) without turning into a solid. In other words, it's a valid surface quilt.
For example if you draw an L-shaped sketch curven and extrude it, you would get a perfectly acceptable surface quilt with 2 faces. If you run "Validate" on that body it would not report any errors.
If you use the Stitch command and pick one or more bodies all the open edges would show up in red. Use that command to find the "holes" that need to be closed up. There are typically two ways to close these holes:
1. Stitch adjacent quilts (or unstitched surfaces). You might have to relax the tolerance. (Though Validate also does stitching, I use the Stitch command for explicit stitching.)
2. Create a patch surface, which is then stitched in.
You cannot stitch a surface in to a solid. Rather than trying to add to a solid, I typically create a new component and move the solid into that component and hide it. The model may actually consist of multiple solids, so your final objective may be several solid bodies rather than a single solid body.
BTW, you could use Sculpt to add a "cell" defined by the surface (normally a quilt that envelopes a volume). This is complicated stuff that you might want to avoid for now.
Sometimes the "intersecting surfaces" are reported wrong. If you suspect that, use Checking Level = Basic to skip intersection checking.
Anyway, as I said earlier, complicated model repair is an "art" where experience helps. Sometimes a model can be so corrupted that it might be easier to recreate it.
I did not understand the difficulties you faced after converting to a solid. Are you not able to create a hole?