Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.
Is there a way to ignore fetures in a mill volume? i.e. I want to cut the perimeter of a part but not put the holes in it... can I have it skip the holes?
You cancreate the mill volume so that when you Trim the reference model, the holes do not show. You can also Modify a mill volume and add features, that "remove" the holes from thevolume.
Do I exclude the holes after I have created the volume? When I go into modifle my volume I have an option called "Gather" .... This seems to be the only thing close to excluding features. It gives me the option to "Fill". Am I headed in the right direction? I am not getting anywhere with this though. BTW I am on Pro 2001.
First thing to remember, is that the mill volume is a protrussion that is exactly the opposite of the part. What is a hole in the part, will be a "boss", or protrussion in the mill volume. To get rid of a boss in a part, you would create some kind of cut. You got to do the same thing in the mill volume. To do this, select modify you mill volume. Now select sketch, and remove. Now pick the type of cut that you want, (extrussion, revolve, sweep, blend,etc.).
Sometimes it helps if the only thing on the screen, is the mill volume. This lets you see what it is you need to "cut away" from it. To do this, go into "component display" and blank all of the models in the assembly. Now you can create your cuts by using the surfaces and/or edges of the mill volume as your references.
Why dont u supress the hole features?? if u want to make holes too, then create a simplified rep and supress holes in it, then make two separate files for manufacturing, one with that simplified rep and another with master rep.
This trick is much easier if u use a window insted of volume. there is an option called close loops in sequence setup menu.it is only applicable for windows. thru this option u can select all the loops u want to avoid from machining.
but one thing is that u cant perfom a local restmilling for this after this operation because it doesnt take the closed loops in account.
I don't know if you guys are still viewing this thread.
i tried the mill volume thing, not the window, and I can't get it to work.
See if I am doing this correctly...
from the Menu Manager...MFG SETUP > Mfg geometry > Mill Volume > Modify Volume > then I select my volume...
... skecth > remove > (Extrude and Solid are highlited) > DONE
Then I go through the sketching parameters... One Side > select my plane (which is the "boss" part of my mill volume, select the sketching reference, as usual.
Now, I skectch a circle around the boss feature that I want to cut away. Then, for the direction,the arrow is pointing to the inside of my circle, (meaning I want that circle cut away), thenselect up to surface and the surface that is at the bottom of the boss. Then OK.
NOW... I see the feature that I created, but I also see the "hole" that I am trying to remove from the mill volume. The menu is now at the point where it lists "gather, Sketch, Rename..." etc. so I click Done/Return, then Done/Return, then Done/Return (as Pro-E always is...lol).
SO, the cut shows up in my model tree right under "Protrusion, Trim, Offset". I can see the cylinder that I created, but the hole is still there. AND, the toolpath still cuts the detail into the hole.
<?:namespace prefix = v ns = "urn:schemas-microsoft-com:vml" />View attachment 2289</v:stroke></v:f></v:f></v:f></v:f></v:f></v:f></v:f></v:f></v:f></v:f></v:f></v:f></v:ulas></vath><?:namespace prefix = o ns = "urn:schemas-microsoft-comfficeffice" /><o:lock aspectratio="t" v:ext="edit"></o:lock></v:shape>
<DIV align=left>
Here is a pic of the part. Well, notthe part; the volume that was trimmed to the part.The central littleknob is the"boss" on my volume. The part that's pointing "up" is the bottom of the hole. I am trying to use the bottom of the hole as my skecthing surface and build the extrusion "down" to the top edge of the hole.</v:image>
</v:image>
Sorry, I don't know how to upload the file for anyone else to expiriment with.</v:image>
</v:image>
</v:image>
</v:image>
</v:image>
</v:image>
</v:image>
</v:image>
</v:image>
</v:image>
</v:image></v:shape></DIV>
View attachment 2290
Here is what my sketched "cut" looks like. But when I regenerate the file, it does not remove the hole. But it still is in the model tree under the protrusion, like I stated before.
Yes, I did this again to be sure I selected 'remove".
Can you "zip" the models and manufacturing files and upload them? I would like to take a closer look at your problem. I am using Wildfire 1, so I should be able to read your files from 2001.
You upload "zipped" files by picking the "floppy disk" button that is just to the right of the "upload picture" button. Edited by: appinmi
Actually, I am using WF2. But, I have tried this since my last post on other volumes and it works slick. I wonder if there might have been some geometry problems with that particular one.
The other guys in the office where I work have started using this technique, also. They really like it.
Great tip. I'll use it often.
I have always excluded surfaces that I dont want to mill in a volume, but I have always had the problem of the cutter still finishing the bottom surfaces (ifthey arehorizontal). ThenI would have to go into 'build cut' and exclude the region (if I could) or try to exclude that particular slice (if I could).
As you can imagine, changing the actual volume is a much faster and cleaner way to go!
I do that quite a bit. And it does work well in a semi-finsh situation. (Although, I have seen quite a few times where a negative bottom_stock_allow does not achieve the correct results. I usually use an axis shift in those situations and leave the bottom_stock_allow at zero)
However, what I was considering was a finishing pass that skips regions, basically. That way I can finish the majority of a part and then come back and finish the smaller areas with smaller tool.
Another thing to consider is that I am programing very small, detailed carbon. I work for a plastic injection mold maker; not production... more like a prototyping shop. I am not well versed in programing steel, but I have found that keeping cutters out of specific areas when milling details into carbon is very important. Chatter marks and deflection are a big issue when cutting a .0005" tolerance (or less) part.
Another solution is to MODIFY the mill volume and "offset" the surfaces that you want to leave stock on. This way the cutter cannot finish these surfaces.
Are you talking about offsetting surfaces that are not the outside of the mill volume? I routinely offset the four outside surfaces (of a rectangular volume, obvoiusly) so that my cutter will mill the entire volume, (I assume that is pretty common practice), but I have never offest surfaces such as a pocket or drafted surface within the volume. Is that what you mean? Sounds interesting... never really thought about that one...
This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
By continuing to use this site, you are consenting to our use of cookies.
ath><?:namespace prefix = o ns = "urn:schemas-microsoft-com