Hello
You do not specify the SW version or the type of screw.
On SW2017, with the drilling wizard, for a screw hole you can ask to have an input and output chamfer (you have to go to the very bottom of the feature manager. it also works for F/90 and CHC holes.
So there's no need to go through advanced drilling.
Hello
I have the impression that you are looking for the command assistance for drilling => type of drilling/ milling =>end condition/ blind.
In this case, you will need to use countersunk screws. Useful for bulking or finishing.
Cdt
Details:
SolidWorks 2019 SP4
For:
- Centering holes diam 6. I only have the milling of the upper side, not the lower one...
- M8 clearance. I only have the milling of the upper side, not the lower one...
Maybe I don't know the rule of use of face milling... Does this have to be done on the side where the screw is inserted or on the side where it comes out?
Hello @Charlesir
The notion of a centering hole doesn't make sense in SW since it's a model of the part after machining.
As @AperrO says, the drilling assistance function offers almost all possibilities, combined or not.
(see attachment)
Kind regards
Weird, I'm on SW17 and I have this:
Could you take a screenshot of your feature manager (possibly in 2 times to get the whole thing)?
@Zozo_mp: SW proposes a category of hole called "centering hole" which is recognized during drawing and causes the automatic insertion of a symbol:
Personally, I use it to locate the pin holes. It's clearer in the Model Tree.
Hello
I confirm what says @stefbeno on SW2017 the option is accessible for all models.
You have to check the inner side to have a chamfer on the opposite side of the one used for the drilling function.
Kind regards
@Stefbeno
Thanks for the info ;-) it must have been twenty years since I last made centering holes and even less now with CNCs.
However, I remember that in the past, we made two centering holes which served as a zero marker on the Hauser time clocks. It's true that at the time, doing several large centers on a milling machine was a feat. hence the time clocks.
It's a veteran I know ;-) ;-) ;-)
Hi all
Yes excellent I don't know, I use the chamfer function ...
But this is better.
Thank you.
@+.
Here's what I have for the passage of an M8 screw. I only have the milling of the top side available. For the centering holes, the same thing.
For me, the milling of the upper side (well the chamfer that is done), it's the little extra that allows me to say that the designer has thought of everything :=). It's especially practical for inserting screws/pins and avoiding a burr...
Any ideas about what's going on?
Hello@charlesir
I have trouble following you or at least hard understanding your PB. ;-) (don't bang your head! )
Here is an image of three types of holes made with one function at a time and in one go with the drilling assistance function: which offers many possibilities. See the attachment
Kind regards
Hello
Do you have complex shapes? This could be a problem.
Have you tried on a plate-type part, like the example of zozo-mp?
Cdlt
Sorry for the 2 identical posts. The site was buggy this morning
Hello
Have you tried it on a flat piece? (Example zozo-mp)
If the part is complex it could be a problem.
Cdlt
Hello
@ yannick.petit : a priori simple shapes, I'm on bent sheet metal in my case.
@Zozo_mp : sorry if I'm not clear. I am looking to do milling on the upper and lower sides when I make a hole (screw passage, centering, tapping, ...) in order to best guide the insertion of screws/pins/... My problem is that I can't find the options (sup and inf face milling). Sometimes the option is there, sometimes not... Regarding the screws I use, they are CHC screws, so it is not possible to make a blade for countersunk head as you showed in your screenshot. In PJ what I want to do on either side of my hole, my problem being that on the latter, I can only do the milling of the upper face, no option for the lower face. At the same time it makes machining quite complex. I hope to be clearer with my explanations!
Hello
It's strange, since this option exists (for a while) I have never encountered your problem.
Maybe a registry key problem?to check:
Close Solidworks
Go to regedit (start, run regedit) and then rename:
HKEY_CURRENT_USER\Software\Solidworks\SolidWorks .... depending on the version you want to reset.
When you restart SW, you will have the "factory" settings
If you want to find the previous settings, delete the created key and replace it with the old one
Have you contacted your Hotline? maybe a Solidworks version bug?
Cdlt
Hello
I just got support on the phone (for another issue) and got my answer.
When I change the end condition (through everything, next surface, ...) the "problem" disappears. So I can do both a top side and a bottom side milling. The caller explained to me that SolidWorks does not consider this a bug, but a limitation in functionality. They realized that the upper and lower sides were not trivial to use and this caused a lot of losses on graphics performance ... So much for the story!
@ charleslr ,
I validated I realized that doing a subtraction or extrusion by putting "up to" rather than one-eyed with a distance took me more time to rebuild.
may the force be with you.
Hello @Charleslr
Can you please close the topic
Kind regards
hello @tous
Very niceanswer ; -) thank you for participating;-)
Cdlt