All,
I am working with a user who has stumbled across an odd scenario. When creating a part, he will create only a portion of the features for the part and then mirror them to create the rest of the parts. However, when placing punches, we have noticed that when mirroring flanged features with punches on them, the punch features and their center points become misaligned in the flat pattern and in the flat pattern view in an Inventor drawing. However, if the entire part is modeled, then the punches put in and mirrored, things appear to work fine. I have tried this in Inventor 2013 and in 2015 and the behavior is the same. Has anyone run into this before? Is there something that we are missing? Thanks in advance for any assistance and have a most blessed day!
Peace,
Pete
Solved! Go to Solution.
Solved by mcgyvr. Go to Solution.
Hi,
A few things...
1) I would look at the Punch Tool used to create iFeature2. It may be trying to reference something that causes Inventor to produce the irregular result. Can you go back to the original part used to create that tool? Look at the sketches and see if you are pulling in geometry you really shouldn't. You might compare material thickness in the orginal punch tool IPT. I've seen strange things happen when the tool expects one thickess but you use it with another. Make sure the punch tool IPT references the sheetmetal "Thickness" variable, not a specific value.
2) I was surprised to see a punch tool used to create a hole. I am not a press programmer and I imagine there are a bazillion ways to program a press. I thought the software would see that hole and select the Ø0.375 hole tool from your library. As it's drawn, the part doesn't have the holes in the flat. It does show the outline of the tool, perhaps that works too? I'm just asking to see if there is a new workflow that I can learn.
3) I noticed the Mirror features each select all the individual features. I suggest mirroring the whole solid instead. That is a little more...uhm...robust, in my opinion. I encourage all my users to use that functionality as often as possible.
-Brian
yes.. I've had the mirrored features created by a punch tool completely disappear in models (rebuilding the part brings them right back though) as well as the same problem you've had.. Its always in how the punch tool was created (and a bit of a buggy issue with the software).
I actually have an ilogic rule that runs on all my sheet metal parts to do a rebuild (before save event trigger).
Hi!!
Can you put here this " Rebuild" code? I Think i will use it also!!!
@CCarreiras wrote:
Hi!!
Can you put here this " Rebuild" code? I Think i will use it also!!!
Its just this and I called it "rebuild before save" and I assigned it to the "before save" event trigger.
ThisDoc.Document.Rebuild()
That was a good idea, but the Rebuild did not help me in this case. I am in the middle of something right now, but have a short break, so I wanted to pass along my base model to you, that I used to create the punch iFeature. Please let me know if I did anything incorrectly. Unfortunately, the forum won't let me post the .ide file, so this is as close as I can get. If you have any questions, please do not hesitate to contact me. Hope all is well and have a most blessed day!
Peace,
Pete
out of curiosity.. Why are you using a punch tool for a single round hole?
Just to tie it to the punch ID maybe?
Mostly, I am doing this because that seemed to be what the user was doing. I figured for the workflow on feature versus two wouldn't make a difference, so I am created the round punch hole in the interest of time. You make an interesting observation and it would be useful to tie this to a specific punch tool. In all honesty, I hadn't made a punch iFeature in a while, so thought it would be good to practice up too.
blair, I thought I did use a sheet metal feature? I certainly intended to anyway. I open up a new sheet metal.ipt template, created a face, created a sketch, placed a centerpoint, drew the circle and then used the Cut feature to create the hole. Then I published the iFeature and did use the depth of Thickness. While not conciously thinking about where or not a sheet metal feature or standard feature would matter, I elected to go down the sheet metal feature route. Do you think there might have been something wrong with my approach?
Frankly this has been an issue with Inventor for a long time.. It really just gets confused sometimes when mirroring punch tools.. Frankly the way that whole part was constructed is kind of "goofy" in that they model one corner of the sheet metal part then mirror then mirror again.. Just seems like a weird method to me and combine that with Inventors ability to get confused with mirrored punch tools and you just run into the perfect storm.
If that part was modeled without all those mirrors I'd suspect that you wouldn't ever see the problem again.
I'd just let the user know to try to avoid excessive mirroring with punch tools.
mcgyvr,
I couldn't agree more and have advised the user to not mirror the punch tools, mostly because I couldn't get it to work either. It is an odd workflow, which I believe I also mentioned and certainly will if I haven't yet. I can see doing this for a complicated sheet metal feature, but the simple flanges really could be accomplished better without the mirror. Anyway, you pretty much have answered my question. While I agree that this is a "goofy" workflow for this type of part, Inventor should be able to handle the mirroring of the features. Really appreciate yours and everyone's input and will simply report this to the feedback section. Hope all is well and have a most blessed weekend!
Peace,
Pete
Hi! I cannot say there is anything wrong with the way the sheet metal part is modele. The features are legitimate operations. It looks like a bug to me. It seems that the center mark and the form punch are placed in the right place. But, the 2D represetation on one mirror side is wrong in flat pattern. I am sending it in as a defect for further investigation.
Thanks!
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